Tutorials proteus schematic

PROTEUS DESIGN
SUITE
Getting Started Guide

COPYRIGHT NOTICE
© Labcenter Electronics Ltd 1990-2019. All Rights Reserved.
The Proteus software programs (Proteus Capture, PROSPICE Simulation, Schematic Capture
and PCB Layout) and their associated library files, data files and documentation are copyright ©
Labcenter Electronics Ltd. All rights reserved. You have bought a licence to use the software on
one machine at any one time; you do not own the software. Unauthorized copying, lending, or
re-distribution of the software or documentation in any manner constitutes breach of copyright.
Software piracy is theft.
PROSPICE incorporates source code from Berkeley SPICE3F5 which is copyright © Regents of
Berkeley University. Manufacturer’s SPICE models included with the software are copyright of
their respective originators.
The Qt GUI Toolkit is copyright © 2012 Digia Plc and/or its subsidiary(-ies) and licensed under
the LGPL version 2.1. Some icons are copyright © 2010 The Eclipse Foundation licensed under
the Eclipse Public Licence version 1.0. Some executables are from binutils and are copyright ©
2010 The GNU Project, licensed under the GPL 2.
WARNING
You may make a single copy of the software for backup purposes. However, you are warned
that the software contains an encrypted serialization system. Any given copy of the software is
therefore traceable to the master disk or download supplied with your licence.
Proteus also contains special code that will prevent more than one copy using a particular
licence key on a network at any given time. Therefore, you must purchase a licence key for
each copy that you want to run simultaneously.
DISCLAIMER
No warranties of any kind are made with respect to the contents of this software package, nor
its fitness for any particular purpose. Neither Labcenter Electronics Ltd nor any of its employees
or sub-contractors shall be liable for errors in the software, component libraries, simulator
models or documentation, or for any direct, indirect or consequential damages or financial
losses arising from the use of the package.
Users are particularly reminded that successful simulation of a design with the PROSPICE
simulator does not prove conclusively that it will work when manufactured. It is always best to
make a one off prototype before having large numbers of boards produced.
Manufacturers’ SPICE models included with PROSPICE are supplied on an ‘as-is’ basis and
neither Labcenter nor their originators make any warranty whatsoever as to their accuracy or
functionality

TABLE OF CONTENTS
COPYRIGHT NOTICE.................................................................................................................. 1
© Labcenter Electronics Ltd 1990-2019. All Rights Reserved................................................. 1
WARNING................................................................................................................................ 1
DISCLAIMER ........................................................................................................................... 1
TABLE OF CONTENTS ............................................................................................................... 3
SCHEMATIC CAPTURE TUTORIAL........................................................................................... 1
INTRODUCTION...................................................................................................................... 1
Creating a New Project ............................................................................................................ 2
Guided Tour ............................................................................................................................. 6
Zooming ................................................................................................................................... 7
Panning .................................................................................................................................... 8
Visual Aids to Design ............................................................................................................... 9
Keyboard Shortcuts.................................................................................................................. 9
Display Options ........................................................................................................................ 10
Design Overview ...................................................................................................................... 12
General Description ................................................................................................................. 12
Circuit Description .................................................................................................................... 13
Basic Schematic Entry ............................................................................................................. 14
Selecting Parts from the Library............................................................................................... 14
Placing Objects on the Schematic ........................................................................................... 19
Wiring Up.................................................................................................................................. 23
Power Connections .................................................................................................................. 27
Part Labels and Annotation...................................................................................................... 30
Timesaving Techniques & Block Editing.................................................................................. 32
Multi-Sheet Designs and Connectivity ..................................................................................... 36
Adding Sheets to a Design....................................................................................................... 36
Naming, Ordering and Navigating Sheets ............................................................................... 37
Connectivity between Sheets................................................................................................... 40

Gateswap ................................................................................................................................. 42
Preparing for PCB Layout ........................................................................................................ 44
Packaging Considerations........................................................................................................ 44
To view the package associated with a component: ............................................................... 44
To change a package on a component.................................................................................... 45
To change a package on all components of a particular type .................................................46
Connectivity Considerations..................................................................................................... 48
To specify a new net class....................................................................................................... 49
Design Verification.................................................................................................................... 50
The Design Explorer................................................................................................................. 50
Assembly Variants.................................................................................................................... 54
Bill of Materials ......................................................................................................................... 56
Printing ..................................................................................................................................... 63
Library Parts ............................................................................................................................. 64
Creating New Devices.............................................................................................................. 70
Graphics and Pins .................................................................................................................... 71
Adding Footprints ..................................................................................................................... 78
Adding Properties..................................................................................................................... 82
Attaching a Datasheet .............................................................................................................. 84
Indexing and Library Selection ................................................................................................. 85
PCB LAYOUT TUTORIAL............................................................................................................ 87
Introduction............................................................................................................................... 87
Overview of the Layout Editor .................................................................................................. 87
The Main Window..................................................................................................................... 88
The Control Bar ........................................................................................................................ 89
Navigation................................................................................................................................. 91
Visual Aids to Design................................................................................................................ 91
Display Options ........................................................................................................................ 92
Graphics Mode ......................................................................................................................... 92
Opacity ..................................................................................................................................... 92
Auto-Pan Animation.................................................................................................................. 93
Highlight Animation................................................................................................................... 93
Multi-Sampling (Anti-Aliasing) .................................................................................................. 94

Displayed Layers Dialogue ...................................................................................................... 94
Component Placement............................................................................................................. 96
Components and Packages..................................................................................................... 96
The Board Edge ....................................................................................................................... 97
Layer Stackup and Drill Spans................................................................................................. 100
Work Area, Co-ordinates and Snap ......................................................................................... 102
Placing Components and the Ratsnest.................................................................................... 105
Mounting Holes and Pad Styles............................................................................................... 112
Design Rules and Net Classes ................................................................................................ 117
Design Rules............................................................................................................................ 118
Net Classes.............................................................................................................................. 120
Keepout Areas.......................................................................................................................... 123
Design Rooms.......................................................................................................................... 126
Routing the Board .................................................................................................................... 128
Placing a Route Manually ........................................................................................................ 129
Panning and Zooming.............................................................................................................. 133
Placing Anchors....................................................................................................................... 133
Getting Stuck / Re-routing while routing .................................................................................. 133
Placing Vias ............................................................................................................................. 133
Object Hugging ........................................................................................................................ 134
Abandoning a Route ................................................................................................................ 134
Making Connections ................................................................................................................ 134
Editing a Route......................................................................................................................... 137
Layer Pairs and Manual Routing.............................................................................................. 137
Basic Auto-Routing................................................................................................................... 140
Length Matching Routes .......................................................................................................... 142
The Selection Filter .................................................................................................................. 144
Advanced Auto-Routing ........................................................................................................... 147
Netlists and Design Changes................................................................................................... 150
Live Netlisting........................................................................................................................... 151
Batch Netlisting ........................................................................................................................ 152
Annotation ................................................................................................................................ 153

Schematic to PCB.................................................................................................................... 153
PCB to Schematic.................................................................................................................... 154
General Netlisting Rules........................................................................................................... 154
Power Planes and Slots ........................................................................................................... 155
Stitching Zones......................................................................................................................... 157
Nesting and Islands.................................................................................................................. 157
Relieve Pins ............................................................................................................................. 158
Exclude Tracking...................................................................................................................... 158
Suppress Islands...................................................................................................................... 159
Allow Nesting ........................................................................................................................... 159
Slots ......................................................................................................................................... 159
3D Visualisation........................................................................................................................ 161
Basic Navigation....................................................................................................................... 162
Bareboard View and Height Clearances .................................................................................. 162
Custom Views........................................................................................................................... 163
3D Models (STEP/IGES).......................................................................................................... 164
Live Update .............................................................................................................................. 165
Board Output Options............................................................................................................... 166
APPENDIX: Creating New Packages....................................................................................... 170
Library Importer ........................................................................................................................ 170
Drawing the Footprint ............................................................................................................... 170
Circular Pad Placement............................................................................................................ 178
Packaging the Footprint............................................................................................................ 180
3D Visualisation........................................................................................................................ 181
VSM TUTORIAL (Interactive)...................................................................................................... 183
Introduction – Interactive Simulation ........................................................................................ 183
Requirements ........................................................................................................................... 184
Project Setup ............................................................................................................................ 184
Compiler Configuration............................................................................................................. 185
Running a Simulation ............................................................................................................... 187
Important Notes ........................................................................................................................ 190
Writing Firmware ...................................................................................................................... 191
Active Popups........................................................................................................................... 194

Basic Debugging ...................................................................................................................... 198
Important Notes........................................................................................................................ 201
The Watch Window .................................................................................................................. 201
Hardware Breakpoints.............................................................................................................. 205
Interactive Measurements........................................................................................................ 207
Graph Based Measurements ................................................................................................... 211
Further Reading....................................................................................................................... 218
Diagnostic Messaging .............................................................................................................. 218
VSM TUTORIAL (Graphs)........................................................................................................... 223
Getting Started ......................................................................................................................... 223
Generators ............................................................................................................................... 224
Probes ...................................................................................................................................... 226
Graphs...................................................................................................................................... 227
Simulation................................................................................................................................. 231
Taking Measurements.............................................................................................................. 232
Using Current Probes............................................................................................................... 235
Frequency Analysis.................................................................................................................. 236
Swept Variable Analysis........................................................................................................... 240
Noise Analysis.......................................................................................................................... 242

1
SCHEMATIC CAPTURE TUTORIAL
INTRODUCTION
The aim of this tutorial is to take you through the process of entering a circuit of modest
complexity in order to familiarise you with the techniques required to drive the schematic
capture module in Proteus. The tutorial starts with the easiest topics such as placing and wiring
up components, and then moves on to make use of the more sophisticated editing facilities,
such as creating new library parts.
An accompanying tutorial in the PCB module then continues the project development using the
completed schematic drawn in this tutorial.
For those who want to see something quickly, DSPIC33_REC_SCHEMATIC.pdsprj contains the
completed tutorial circuit but no layout while DSPIC33_REC_UNROUTED.pdsprj and
DSPIC33_REC_COMPLETE.pdsprj both contain a completed schematic and a PCB. All of
these projects can be loaded from the Open Sample command on the Proteus 8 home page
under the tutorials category.
Note that throughout this tutorial (and the documentation as a whole) reference is
made to keyboard shortcuts as a method of executing specific commands. The
shortcuts specified are the default or system keyboard accelerators as provided
when the software is shipped to you. Please be aware that if you have configured

LABCENTER ELECTRONICS LTD.
2
your own keyboard accelerators the shortcuts mentioned may not be valid.
Information on configuring your own keyboard shortcuts can be found in the
General Concepts section of the Documentation.
Creating a New Project
We shall assume at this point that you have installed the Proteus 8 software package.
To start the software, click on the Start button and select Programs, Proteus 8 Professional and
then the Proteus 8 application. The main application will then load and run and you will be
presented with the Proteus home page.
If you have a Demonstration copy of the software you can start the Proteus
application via the Proteus 8 Demonstration tab from the Start Menu.
In order to create a schematic we must first create a project. Since this tutorial is partnered with
the PCB tutorial we will create a project for schematic/PCB.
Start by pressing the new project button near the top of the home page in Proteus.
On the first page of the wizard specify a name and path for the project.
We need a schematic so check the box at the top of the next step and then choose the default
template.

Schematic Capture
3
Similarly, we need a layout so check the box at the top of the layout page and again choose the
default template.
The next screen allows us to define the layer stack for our PCB. Since we will be designing a
simple two layer board there is no configuration necessary here.
For multi-layer PCB's the stackup wizard button would be used to define the
number of copper layers, cores and pre-preg's. This is discussed in more detail in
the accompanying PCB tutorial.
The next screen is for configuration of drill spans. Again, for our proposed 2-layer board the only
possibility is thru-hole so there is no action required.

4
The final screen in the PCB configuration is simply a preview of a PCB cross section that
displays visually what has been set up in the previous screens.
We are not simulating the design so leave the firmware page blank and continue on to the
summary which should look like the following:

Schematic Capture
5
Click on the finish button to create the project.
A schematic template can contain sheet size, colour scheme, company logo, header
block and various other aesthetic presets. Further information can be found in the
Templates chapter of the reference manual.
A PCB template can contain board edge, mounting holes, design rules, layer stack and
various other technology information. Refer to the Templates chapter in the PCB
documentation for more information.
The configuration of the Layer Stack and Drill Spans is really important for multi-layer
PCB's and is discussed in some detail in the reference manual.
The project will open with two tabs, one schematic capture and the other for PCB layout. Click
on the schematic tab to bring the Schematic module to the foreground.

6
Guided Tour
The largest area of the screen is called the Editing Window, and it acts as a window on the
drawing - this is where you will place and wire-up components. The smaller area at the top left
of the screen is called the Overview Window. In normal use the Overview Window displays, as
its name suggests, an overview of the entire drawing - the blue box shows the edge of the
current sheet and the green box the area of the sheet currently displayed in the Editing Window.
However, when a new object is selected from the Object Selector the Overview Window is used
to preview the selected object - this is discussed later.
Schematic Capture Window
If you don’t like the default layout of the toolbars you can pick them up and dock them on any of
the four sides of the application. Similarly you can move the Object Selector & Overview
Window pane across to the right hand side of the application by dragging the end of it all the
way across to the other side.
Toolbars and menu options will switch according to which tab is active (at the front).
Throughout this tutorial when we refer to an icon or a menu command we are
assuming that the schematic tab is active.
Right clicking the mouse either in the Object Selector or in the Overview Window will provide a
context menu, including the option to ‘auto hide’ the left hand pane. This is extremely useful if
you want to maximise the editing area of the application. When enabled the Object Selector and
Overview Window will be minimised to a ‘flyout bar’ at the left (or right) of the application by
default and will appear either when the mouse is placed over the bar or when the mode of
operation is changed by selecting a different icon.

Schematic Capture
7
Auto hide the Object Selector Device Mode Icon
Navigation of the view displayed in the Editing Window takes two forms; adjusting the scale of
the drawing (zooming) and adjusting the area of the drawing displayed (panning). These
techniques are somewhat intertwined and are discussed in more detail below:
Zooming
There are several ways to zoom in and out of areas of the schematic:
Point the mouse where you want to zoom in and out of and roll the middle mouse button
(roll forwards to zoom in and backwards to zoom out).
Point the mouse where you want to zoom in or out of and press the F6 or F7 keys
respectively.
Hold the SHIFT key down and drag out a box with the left mouse button around the area
you want to zoom in to. We call this Shift Zoom
Use the Zoom In, Zoom Out, Zoom All or Zoom Area icons on the toolbar.
Zoom Icons
The F8 key can be used at any time to display the whole drawing.
The Shift Zoom and the middle mouse zoom techniques can also be used over the
Overview Window. That is, you can position the mouse over the Overview Window
and either roll the middle mouse button or use Shift Zoom to navigate in or out of an
area of the schematic.

8
Panning
As with zooming, there are a number of options for panning across the editing window.
Click on the middle mouse button to enter track pan mode. This puts the schematic in a
mode where the entire sheet is picked up and will move as you move the mouse. The
track pan cursor will indicate when you have entered this mode. Left click the mouse
again to exit track pan mode.
To simply 'pan' the Editing Window up, down, left or right, position the mouse pointer over
the desired part of the Editing Window and press the F5 key.
Hold the SHIFT key down and bump the mouse against the edges of the Editing Window
to pan up, down, left or right. We call this Shift Pan.
Should you want to move the Editing Window to a completely different part of the
drawing, the quickest method is to simply point at the centre of the new area on the
Overview Window and click left.
Use the Pan Icon on the toolbar
Note that when using the track pan method above you can also zoom in and out by
rolling the mouse wheel. So, click the middle mouse button to pick up the sheet and
move the sheet by moving the mouse and zoom the sheet by rolling the middle
mouse button. Left click to 'drop' the sheet and exit track pan mode.
It is well worth spending a few moments familiarising yourself with navigation in Proteus - it is
after all one of the most common operations you will perform. In particular, learning to use the
middle mouse button both for track pan and for zooming will save you time during schematic
design.
A grid of dots or lines can be displayed in the Editing Window as a visual aid using the Grid
command on the View menu, or by pressing 'G' to toggle the grid from ‘dots’, ‘lines’ or ‘off, or by
clicking the Grid Icon on the toolbar. The grid helps in lining up components and wires and is
less intimidating than a blank screen. If you find it hard to see the grid dots or lines, either adjust
the contrast on your monitor slightly (by default the grid is displayed in light grey) or change
their colour with the Set Design Defaults on the Template menu.
Below the Overview Window is the Object Selector (sometimes known as a 'parts bin') which
you use to select devices, symbols and other library objects. We'll familiarise ourselves further
with using the Object Selector later.
Finally, at the bottom of the screen is the co-ordinate display, which reads out the co-ordinates
of the mouse pointer when appropriate. These co-ordinates are in 1 thou units and the origin is
in the centre of the drawing
Origin Co-ordinates

Schematic Capture
9
Note that Proteus allows you to reposition all the icon toolbars as well as
move/resize the Object Selector/Overview Window. Do be aware however, that this
documentation refers to all the rebars and windows in their default locations.
Visual Aids to Design
Proteus is designed to be as user friendly as possible and provides two main ways to help you
see what is happening during the design process – objects are encircled with a dashed line or
‘twitched’ when the mouse is over them and mouse cursors will change according to function.
Essentially, the object-twitching scheme tells you which object the mouse is over (the ‘hot’
object) and the mouse cursor tells you what will happen when you left click the mouse on that
object. While extremely intuitive, a summary of cursors used, together with their actions, is
provided below:
Cursor Description
Standard Cursor - Used in selection mode when not over a 'hot' object.
Placement Cursor - Placement of an object will commence on a left click of the
mouse.
Hot Placement Cursor - Appears green when placement of a wire is available on left
click of the mouse.
Bus Placement Cursor - Appears blue when placement of a BUS is available on left
click of the mouse.
Selection Cursor - Object under the mouse will be selected on a left click of the
mouse.
Move Cursor - The currently selected object can be moved.
Drag Cursor - The wire or 2D graphic can be dragged by holding the left mouse
button down
Assignment Cursor - When over an object (having set the Property Assignment Tool)
You can assign the property by left clicking the mouse button.
We will see more of the different cursor types throughout the course of the tutorial.
Keyboard Shortcuts
For those customers who prefer to invoke commands and dialogues via the keyboard Proteus
provides a comprehensive and flexible scheme for assigning shortcuts. The dialogue form is
invoked from the System Menu – Set Keyboard Mapping command, where all commands and
operation modes can be accessed from the combo box at the top. Simply select the command
you want, apply a key sequence and assign it to that command

10
Keyboard Mapping Dialogue Form
While there are few limits on shortcuts, a few standard windows accelerators are
restricted as they are global across the entire Proteus system (e.g. CTRL+S for
save).
Display Options
Proteus is capable of harnessing the power of your computers graphics card to speed up
operation and present a crisp and smooth display. However, as not all machines have sufficient
graphics cards the software is also capable of using Windows to perform display and graphical
operations. The available modes of operation are called:
Windows GDI Mode.
OpenGL Hardware Accelerated Mode.
Direct 2D Hardware Accelerated Mode.
If your graphics card is not powerful enough to support hardware acceleration then Proteus will
simply default to Windows GDI mode. Should your computers graphics card be capable of both
Direct2D and OpenGL the system will default to Direct2D mode as this tends to be more reliably
implemented by graphics card vendors.

Schematic Capture
11
Configuration of the screen display takes place from the Set Display Options on the
System menu. Some of these options are specific to a particular hardware acceleration
technology and will be disabled when a different mode is enabled.
The Set Display Options Form for OpenGL and Direct2D
The first section of the dialogue reports on whether your graphics card will support OpenGL
and/or Direct2D hardware acceleration and, if so, allows you to switch between graphics mode.
The auto-pan section of the dialogue allows you to control distance, smoothness and speed of
pan operations on the schematic. For example, holding down the shift key and bumping the
mouse against the edge of the window will auto-pan the screen.
The highlight animation options allow you to specify the speed at which objects become active
when the mouse is moved over them. The attack rate is the rate at which the object is
highlighted and the release rate is the speed at which the object returns to its default state.
These options are only available in hardware accelerated display modes.
Finally, the multi-sampling combo box allows you to specify the level of anti-aliasing you want
when working in OpenGL mode. The higher the level of multi-sampling the better the anti-
aliasing effect but the more GPU resources are consumed. If you select a level of multi-
sampling which is not supported by your graphics hardware the software will reset the level to
the closest one which your card can handle.
What you get with multi-sampling varies enormously between graphics cards. Some
present extremely smooth text, while with others it looks blurry and on a few it causes

12
display issues. We would suggest you being with multi-sampling off if you choose to work
in OpenGL mode.
Configuration of colours and styles in Proteus takes place from the Template Menu. This
allows to change everything from paper, grid and highlight colours to the thickness and
colour of all the object types used in a design. Please refer to the reference manual
section on Templates for more information.
Design Overview
The circuit we are going to draw is shown below. This is reasonably straightforward schematic
that will nonetheless allow us to cover most of the major features of the Proteus schematic
capture package. Being a real-world design, it will also allow users to follow the design through
the PCB phase of development via the PCB tutorial.
The dsPIC33 Data Recorder Sample Design
General Description
The dsPIC33 Data Recorder Tutorial circuit is a solid state recorder designed to collect three of
the most important environmental variables:
Atmospheric pressure
Ambient temperature

Schematic Capture
13
Relative humidity
A number of low cost silicon transducers with built-in signal conditioning or digital interfaces
have been used for measurement. This reduces the number of components to the minimum
required for dsPIC33 interfacing.
All measurements get periodically stored into a non-volatile, low power memory in row binary
format for later transfer to a host PC either by using a serial terminal or, more properly, a simple
program (not supplied with the project). For the purpose of this project a serial terminal is used.
The circuit is designed to work with a battery for relatively long period in an unattended
environment and, as such, a particular emphasis has been given to optimizing the power
consumption and consequently the battery life. The recorder will sleep most of the time and will
be woken up periodically only to accomplish the required recording operations.
Circuit Description
The following is a block diagram showing the behaviour and interaction of the circuit
components.
Block diagram of the dsPIC Data Reorder Design
We’ll cover the basics of the design construction as we progress through the tutorial but in order
to keep the focus on the practical aspects of using the software, design decisions and theory
will not be discussed in this document.

14
Basic Schematic Entry
We’ll start the tutorial by familiarizing ourselves with the basics of schematic design; picking
components from the libraries, placing them on the schematic and wiring them together.
The design in question is relatively large and there is therefore a reasonable amount of drawing
involved. We provide a completed schematic at the end of this section so, if you feel that you
have mastered the basics at any point, there is no need to continue with drawing the remainder
of the circuitry. We do however urge you to read through the full contents of the documentation
as we introduce important features throughout.
The first thing we need to do is to get the parts from the libraries that we need in our schematic.
Selecting Parts from the Library
You can select parts from the library in one of two ways:
Click on the P button at the top left of the Object Selector as shown below. You can also
use the Browse Library icon on the keyboard shortcut for this command (by default this is
the P key on the keyboard).
Right click the mouse on an empty area of the schematic and select Place – Component -
From Libraries from the resulting context menu as shown below:

Schematic Capture
15
Either of these two methods will cause the Device Library Browser dialogue form to appear.
For reference, the following is a list of all the components we will need for our design:
2N7002 24LC64 AVX0805NPO22P AVX0805X7R1N AVX08055X7R10N
AVX0805X7R100N B82432T1103K000 BAS40 CHIPRES1K CHIPRES10K
CHIPRES20K CHIPRES68K CHIPRES100K CHIPRES100R CHIPRES200K
CONN-H2 CONN-SIL4 CONN-SIL6 CRYSTAL DSPIC33FJ12GP201
JUMPER LED-RED LM285-2V5 LM358 MAX1724
MPX4115 SHT15 TAWD106M025R0600
There are several ways in which we can find and import components from the libraries into the
schematic. In the case of parts where you would know the part name it’s usually best to start the
search with that. Try entering ’2N7002’ into the Keywords field on the Device Library Browser
dialogue form. This gives a direct result and we can then simply double click on the part in the
results list to import it into the schematic. When you do this you should notice that the part now
populates the Object Selector as in the following screenshot.

16
The 2N7002 in the Object Selector
Given that we know the names of all the parts we want we could simply proceed by using this
technique to bring in all the components we need. However, this may not always be the case
and Proteus provides several methods for finding parts in the component libraries. One of the
most intuitive is to use the library browser a little like an internet search engine, typing in
descriptive keywords and then browsing the results to find a specific part. Try this now with the
resistors, typing in ‘1k resistor’ in the keywords field of the library browser dialogue to locate the
CHIPRES1K component (double click on the part in the results list to import into the schematic).
We could similarly search for ‘10k SMT resistor’ to find and insert the CHIPRES10k component
and so on.

Schematic Capture
17
Picking a CHIPRES1K Resistor from the Pick Devices form
Note that there are web search results accessible by clicking on the yellow bar at the bottom of
the search display. This provides free access (you need to register a free account) to over 15
million library parts, meaning that if the part is not included with the installed libraries you can
still source it from this dialogue form.
You can customize the information displayed in the Library Browser’s results list by right
clicking the mouse on the results list. The context menu provides you with options to display
Categories, Sub-Categories, Manufacturer and Library alongside each result.
It may be that we simply want to browse for a specific type of part and/or one available from a
specific manufacturer. To take an example, clear out the contents of the keyword field and then
select the Capacitors Category. In our design we are looking for some Nickel Barrier caps from
AVX so we can further filter the results set by selecting Nickel Barrier from the sub-category
field and AVX from the Manufacturer field. There are still a large number of caps available so
we might type in ‘22p’, ‘1N’, etc. in the keywords field to isolate and select the particular
components we require (AVX0805NP022P, AVX0805X7R1N and so on).

18
Whilst this exercise is a little contrived given that we are starting from a preset list of parts, the
techniques described are flexible enough to allow you to locate any library part quickly. Work
through the full parts list for the design (as provided above) now using one or more of these
methods to find and select the parts into your design. When you are finished you should have
all of the required components in the Object Selector as shown in the following screenshot.
A Full list of required components
For example, if you wanted to search for a specific stockcode you would need to make sure that
the stockcode column was enabled (right click on results list) and then type something like ‘digi
<stockcode>’ to locate the digikey stockcode.
Similarly, if you want to search through only your own library parts, you can simple enable the
library field and then type something like ‘user <partname>’; the user term will filter the results to
the USERDVC library thus reducing the search range to your own libraries.
It is inevitable that at some point there will be parts needed for a project which
aren't supplied in the installed libraries. In such cases you can quickly download
and import the parts free of charge from popular third party vendors such as Ultra-
Librarian, SnapEDA, Library Loader or PCB Library Expert. The process is
discussed in detail in the reference manual and also covered in video format on the
website and our Youtube channel.

Schematic Capture
19
Placing Objects on the Schematic
Having selected the parts we need the next thing is to actually place them on the drawing area
– the Editing Window – and wire them together. You’ll notice from the screenshot that we have
also split the contents of the schematic into logical blocks of circuitry. This is partly aesthetic but
also reduces wiring clutter on the schematic and will allow us to cover the use of terminals to
form connections as we work through the tutorial.
Main Sheet of the dsPIC33 Data Recorder Schematic
We are going to start off simply and complete the block of circuitry comprising the I2C Memory
device as shown below.

20
I2C circuit section
Begin by placing the I2C memory device as follows:
Select the 24CL64 device from the Object Selector.
Left click on the schematic to enter placement mode.
Move the mouse to the desired location for the part, then left click the mouse again to
‘drop’ the part and commit placement.

Schematic Capture
21
Often we need to move parts or blocks of circuitry after placement and now is a good time to
cover the different ways in which we can do that. The procedure for this should be familiar to
most users; we need to select the object(s) we want to move, left depress the mouse, drag to
the new location and finally release the mouse to drop.
We can select an object in several ways as detailed below:
Choose the Selection Icon and then left click on the object. This is a standard technique
found in most graphical applications and will tag any object. Bear in mind when using this
technique that you must change back to component mode for example, when you wish to
perform other actions such as placing components etc.
Right clicking the mouse on an object will both tag the object and present a context menu
containing available actions on that object.
Draw a tagbox around the object by depressing the left mouse button and dragging the
mouse to form a box encompassing the object to be selected. This method will work for
any object (or indeed sets of objects). Sizing handles are provided to allow you to resize
the tagbox in the event that it does not fully enclose the object. This is the technique that
should be used for moving multiple, connected objects or blocks of circuitry.
We’ll get plenty of practice moving things around as we lay out the schematic; for now just use
one of these techniques to move the memory device down towards the bottom left of the Editing
Window in roughly the same position as in the screenshot at the top of the section.
Having placed the memory device, we now need to get the peripheral circuitry down and
oriented correctly. We are going to need two 10k pull up resistors and two 100 Ohm resistors for
the data and clock lines. Additionally, we are going to need to use terminals to achieve
connectivity with power, ground and other sections of circuitry. Begin by selecting the
CHIPRES10k device and click left once on the anti-clockwise Rotation icon (shown below); note
that the preview of the resistor in the Overview Window shows it rotated through 90°.
Using the Rotation Icons with the Overview window

22
Now place the resistor above and to the left of the memory device in the same way as before.
Then, simply left click again on the Editing Window to start placing the second 10K resistor just
beside the first one.
Next, select CHIPRES100R, rotate appropriately (see above) and place two to the left of the
memory device in line with the SCK and SDA pins.
You can also rotate parts 'live' when in placement mode. Left click the mouse once
to enter placement mode (at this point you will see the component outline following
the mouse) and then use the '+' and '-' keys on the numeric keypad to rotate the
component as you are placing it. Left click again to commit the placement in the
normal way.
We use terminals in schematic design simply to terminate a wire and assign a connection. Often
this connection is to either power or ground but it can just as easily be to another wire
elsewhere on the circuit. Terminals allow us both to vastly reduce actual wiring (avoiding
spaghetti schematics) and to make connections between different sheets on the schematic. To
place terminals, start by selecting the terminal mode; this will switch the Object Selector and
provide us with a listing of the available terminal types.
We need a power terminal, ground terminal and also two default terminals for the connections
on the I2C bus. From this stage, placement and orientation are identical to any other object in
Proteus and should now be quite familiar. Place the appropriate terminals in their approximate
locations now, such that the area around the memory device now looks something like the
following
Selecting the Default Terminal
Unless you are fairly skillful, you are unlikely to have got all the components oriented and
positioned entirely to your satisfaction at the first attempt, so now is a good time to practice
moving things around as discussed earlier. In particular note that you can drag a tagbox around
a group of objects to move the lot in one go.

Schematic Capture
23
Components positioned correctly
Similarly, you can clear a selection (or group of selections) either by left clicking in empty space
or by right clicking in empty space and choosing the Clear Selection option from the resulting
context menu
Dragging components
Remember that you can rotate while moving by using the '+' and '-' keys on the numeric keypad.
Wiring Up
Having placed all the requisite components we now need to wire them together. There are three
main techniques used to help make wiring a circuit as simple and quick as possible:
Modeless Wiring
There is no 'wiring mode' in Proteus - wires can be placed and edited at any time, without the
hassle of entering a dedicated wiring mode prior to placement. This means less mouse travel,
less mode switching and quicker development.
Follow-Me Wire Autorouting
After starting to place a wire, the proposed route of the wire will follow the movement of the
mouse orthogonally to the termination point of the wire.

24
Live Cursor Display
The cursor will change as a visual indicator when wiring to show when a wire can be placed,
when a wire can be terminated and when a wire is being placed.
The basic procedure for placing a wire between two pins is given below, using the connection
between the SCK pin of the memory device and the 100Ohm resistor as an example:
Move the mouse over the SCK pin on the memory device - the cursor will change to a
green pen.
Left click the mouse and then move it to the left until it is over the pin of the 100 Ohm
resistor. The wire will follow the mouse and the cursor / pen is white during wiring
Left click the mouse again to commit the connection and place the wire.
The procedure for wiring onto an existing wire is almost identical but there are a couple of items
to note:
You cannot directly start a connection from an arbitrary point on a wire; in our example
you want to start the connections from the pin and terminate them on the wire.
When you terminate the connection on another wire a junction dot will be placed
automatically to complete the connection.
Dragging a wire
If, during a design, you want to make a wire-to-wire connection you must first place a junction
dot on the wire and then wire from the junction dot to the other wire
If you want to adjust a wire after placement (for example, the wire from the SDA pin to the
resistor) then simply right click on the segment you want to move and then either select the
‘Drag Wire’ context menu option or simply depress the left mouse button and drag to the new
location.

Schematic Capture
25
Armed with the above you should now be able to connect up all of the circuitry, so that your
schematic now looks something like the following
Schematic section with all parts / terminals placed
Remember, Proteus provides visual indicators to help you. If the cursor turns green
you can start/stop wire placement.
Connectivity by Touch
The following basic rules of thumb may be helpful:
Iif you are placing the component you can attach to another component, wire or terminal
directly.
If you are dragging the component you can attach to another component pin, junction dot or
terminal.
If you are copy and pasting you can only attach it to a pin end, a bus pin, a junction dot or a
terminal only.
Making Connections with Terminals
The final thing we need to do to complete this block of circuitry is label the terminals. Terminal
naming is extremely important as it denotes the connection to be made. We could name the
terminals in any fashion we liked but sensible names make the schematic more legible and
easy to understand.

26
Terminal connection
Power, Ground and NC terminals are the exception to this rule, although there is no
reason not to label them; an unlabeled power terminal is assigned to the VCC net
and an unnamed ground terminal will be assigned to net GND. A pin connected to
the NC terminal is NC and cannot then be connected on the layout.
Essentially what we are doing by labeling a terminal is making a connection to somewhere else
on the schematic (a terminal with the same name) without placing a physical wire between the
two objects.
As discussed previously, if you are in any doubt, Proteus is flexible enough to present you with
several methods for editing parts - choose your preferred method for editing the terminal from
the following:
Double left click on the terminal.
Right click on the terminal to select it and launch the context menu and then use the Edit
Properties menu option.
Enter Selection Mode, left click to highlight the terminal, then right click to launch its
context menu and use the Edit Properties menu option. Remember to exit selection mode
when you are finished.
Having now launched the terminals dialogue form, type in VDD in the edit field as shown below
and hit ok to exit the dialogue form.
Note that, where appropriate you should always prefix numerical terminal values with a '+'
or '-'. For example, a terminal labelled 12V is ambiguous and you should therefore ensure
it is labelled +12V or –12V.
Finish the job now by editing the other terminals and labeling them appropriately such that your
completed circuit block now looks like the following:

Schematic Capture
27
Schematic section completed
Power Connections
Proteus supports a powerful scheme for making power connections implicitly, thus vastly
reducing the number of wires on the schematic. There are three main concepts involved that we
will discuss in turn below.
Hidden Power Pins
Almost all relevant parts in Proteus have their power pins hidden (not visible on the schematic).
The crucial point to remember is that in such cases is that by default the name of the pin
denotes the net to which it will connect.
If you need all pins to be visible on the schematic (e.g. for auditing purposes) consider
using the library import tool (Library Menu -> Import Part) to bring in the parts you need.
This process is quick and easy and works with library parts supplied from all major
vendors.
Power Rail Configuration
The easiest way to manage power nets and connectivity is through the Power Rail
Configuration dialogue form, which is invoked from the Design Menu. If we do this now we can
see that we have three pre-defined power supplies, namely GND, VCC/VDD and VEE.
Changing the combo box at the top we should also see that the GND net is connected to the
GND supply and that both the VCC and the VDD nets are connected to the VCC/VDD supply.
It’s worth examining how this happened more closely:
The GND net is created by connections to an unlabeled ground terminal.
The VDD net is created by connections to the power terminal labeled VDD.
The I2C memory has two hidden power pins, VCC and GND, which are assigned to nets
bearing their names.

28
Managing power nets and power supplies is a very important concept so we’ll experiment a little
to re-enforce the point. Exit the Power Rail Configuration dialogue form, right click on the I2C
memory part and select Edit Properties from the resulting dialogue form. Next, click on the
Hidden Pins button at the right hand side to view the hidden pins and their net assignments.
Hidden Power pins in schematic components.
Let’s change the power pin to be on net VDD, instead of the default of VCC. If we then exit the
dialog and re-invoke the Power Rail Configuration dialogue and switch to the VDD/VCC power
supply we should see that the VCC net is no longer present (this was the only connection on
our schematic so far).
While we are here and for completeness change the Voltage of the power supply to be 3.3V,
which is actually what we will be using. In PCB Design this is useful only as a reference to
ourselves but actually has significance in the software for simulation purposes.
This exercise, while useful in explaining how to view/change the power nets for individual
components, had no effect on design connectivity. The software is clever enough to assign both
the VCC and the VDD nets to the same supply and the Power Rail Configuration dialogue
allows us to configure our power connectivity at design level.
Returning to the schematic now, edit the VDD terminal (right click, edit properties) and change
the terminal label to ‘MY_POWER_NET’. If you go back to the Power Rail Configuration
dialogue you should see that this is now an unconnected power net (a power net which is not
associated with a power supply).

Schematic Capture
29
Changing the Terminal name
If we were doing this for real, we would now have to select the VSS/VDD power supply and then
click the assign button to map our power net onto the correct supply.
If we had simply removed the label from the power terminal (instead of renaming it),
it would have been designated to the VCC net and again everything would be done
for us.
A final point worth noting is that new power supplies are created automatically when you label a
terminal with a voltage. For example, labeling a power terminal +12V would create a +12V
supply and assign the +12V net to the supply automatically. This means again that no action is
required by the user.
In general usage therefore, the software will handle the assignments of power nets to power
supplies and will create new supplies automatically. However, if you need more flexibility (for
example, an analogue ground and a digital ground) then using terminal labels and the Power
Rail Configuration dialogue gives you the control you need. Please see the reference manual
for more information if required.
Let’s change our terminal label back to VDD for consistency before we move on.
For more information please visit Power Rail Configuration in the Online Help.
Global Power Nets
Power nets and connections are always global on a given sheet on the schematic. By default,
they are also global to the design. However, if you do have a multi-sheet design and you want
separate power supplies on different sheets you can isolate the supplies by un-checking the
Global Power Nets box (Design Menu - Edit Design Properties dialogue form). This means that
you need to explicitly wire through the sheets on the design but not within a given sheet. It is
typically used only for the most complex of designs and is not relevant for the purposes of this
tutorial.

30
Part Labels and Annotation
You should see that all the parts you have placed have both a unique reference and a value. A
unique and sequential annotation is assigned to components as you place them on the
schematic, although you can re-annotate manually if you need to.
You have full control over the position and visibility of part labels – you can change the values,
move the position or hide information that you feel is unnecessary. The discussion below
details how to manipulate part labels on a per component basis.
If you zoom in on any resistor you have placed you will see that Proteus has labelled it with a
unique Reference (e.g. ‘R1) and also with a Value (e.g. ‘10k’). You can edit both these fields
and their visibility via the Edit Component dialogue form. Launch this dialogue form now by
double clicking the left mouse button over the resistor (or using one of the alternative methods
discussed previously).
The Edit Component dialogue form
From the resulting dialogue form you can edit both the part name reference and, in this case,
the resistance. Of more interest to us however, is the visibility options (highlighted in the above
screenshot). It can be useful, particularly in densely populated schematics to hide some details
displayed beside the parts – the tradeoff being that you would then need to edit the part as
above to see its reference and value.
At this stage it is worthwhile familiarising yourself with editing components and hiding and
showing references and values.
Some caution is required when changing part references in this manner. If, for example, you
change ‘R1’ to be ‘R2’ then you will have two parts with the same reference on the schematic.

Schematic Capture
31
This will cause netlist errors when working in the PCB module. If, however, you re-annotate
using the new button on the edit component you are guaranteed a unique part reference.
The 'New' button will automatically assign a new reference
Similarly, the Global Annotator (discussed later in the tutorial) will always avoid duplication of
part references.
As well as the ability to hide part labels you can move them to a more convenient place. This is
commonly used where you might want to place a wire over the current position of the label and
need to free up some screen space. We will try this now with the 'R2' and the '10k' labels on the
pull up resistor, moving them across to the other side of the component body.
Start by selecting the resistor. Now point at the label 'R2' and with the left button depressed,
drag it to its new position to the left of the component body. Then do the same with the '10k’
label.
Dragging a reference

32
Timesaving Techniques & Block Editing
Armed with all of the basic techniques we can now look at the other blocks of circuitry on the
front sheet of the design, practice what we have covered so far and introduce a couple of new
timesaving techniques. Let’s start by drawing the dsPIC33 block as shown here:
dsPIC33 Circuit section
You should be able to tell which components go where by comparing the component names in
the Object Selector to the parts labels on the screenshot above. For clarity however, you can
use the following table as a reference:
C1,C2 AVX0805NP022P X1 CRYSTAL
C3 TAWD106M025R0600 C4 AVX0805X7R100N
R8 CHIPRES10K R9 CHIPRES1K
R10 CHIPRES100R D1 LED-RED
D2 BAS40 JP1 JUMPER
U1 DSPIC33FJ12GP201
Begin by placing and wiring the oscillator and power sections (left hand side) of this circuitry
using the methods outlined in the previous sections. When you are ready we’ll look at the right
hand side, where we can use a couple of additional features to speed up the process.
Proteus has a very useful feature to help with schematic wiring when we are laying out a series
of topologically identical wires. Essentially, it allows us to auto-repeat the last wire placed to
form a new connection.

Schematic Capture
33
Start by rotating and placing a couple of the terminals to the right of the processor.
Terminals belonging to the dsPIC33
Now drag a box around the terminals and select the block copy command; this will allow you to
quickly copy out three more sets of terminals ready for connection. Right click the mouse when
you are finished to exit block copy mode
Block copying Terminals
Wire up the first connection from pin 4 (RB0) of the dsPIC to the terminal exactly as we
discussed previously. Instead of repeating the process for the other seven connections simply
hover the mouse over the next pin down (so that the cursor turns green) and double click. This
will auto-repeat the previous connection, allowing you to rapidly wire up the other lines.
Note that this technique works by placing an identical wire to the one placed directly
beforehand. It follows that the destination must be exactly the same distance away
(i.e. aligned) and that you must perform the operations consecutively
We can now complete this section of circuitry, placing and wiring up the remaining components
and labeling the terminals as per the screenshot at the top of the section. Note that a list of

34
existing terminal label names is available as a drop down list from the Edit Terminal dialogue
form (refer to the section on labeling terminals if you need a reminder).
Drop down list of Terminals
It is highly recommended that you use this where applicable as it avoids the potential to make
typing errors. Remember that terminal names donate connections so care should be taken
during labeling.
You should be getting quite proficient at basic schematic entry now and the other three small
blocks of circuitry on this sheet should present no problem. When you are finished your
schematic should look something like the one below:

Schematic Capture
35
Completed dsPIC33 circuit
If you feel comfortable with the topics we have covered to date, you can skip some
of the drawing and load a pre-supplied completed schematic later in the tutorial
As a final point it is worth re-emphazing that you can re-arrange or move blocks of objects at
any time by tagging a box around them and dragging them to the desired location.
Moving a block of circuitry to the desired location

36
Multi-Sheet Designs and Connectivity
It is increasingly common in larger designs to split the schematic into multiple sheets. This
serves both to reduce clutter on the schematic and also to organize the design into logical
blocks. Proteus fully supports this methodology and we have arranged our tutorial design into
two sheets in order to cover the relevant procedures. The work we have done so far has been
to complete the first sheet (processor, sensors and memory circuitry), meaning we still need to
cover the analog and power circuitry. We’ll do this on a separate sheet.
While beyond the scope of this tutorial it is worth mentioning that Project Clips provide a method
for re-using logical blocks of design and layout. More detail is in the reference manual and a
short tutorial movie is linked on our website.
Also, note that what we are doing here is adding a second sheet at the same level as the first
sheet. Proteus fully supports hierarchical designs where you use sub-circuits to contain logical
blocks. This is discussed in detail in the reference manual.
Adding Sheets to a Design
To add a new sheet to the schematic we simply invoke the command from the Design menu as
shown below.
Creating a new sheet
Try this now to generate the second sheet.

Schematic Capture
37
Naming, Ordering and Navigating Sheets
Before we lay out the circuitry on this sheet we need to do a little housekeeping. While it’s not
necessary it is often helpful to name the different sheets on the schematic and also to order
them in some sensible fashion. We can do both of these things via the Edit Sheet Properties
command on the Design Menu.
The Edit Sheet Properties dialogue form
The Sheet Title is what will be displayed and should therefore reflect the contents of the sheet.
In our case let’s name it ‘Analog, Reference & Power’.
Sheets on the schematic are organized by Sheet Ordinal and by default these are 10, 20 and so
on. A sheet with an Ordinal of 20 will therefore appear behind the first sheet (default Ordinal
10). If you prefer purely numeric nomenclature we can change the sheet name to be ‘2’, to
better reflect its position in the design structure.
The default sheet names may seem inconsistent. This is because Proteus also has
a Master Sheet, present in all designs, which allows the application of a company
logo, revision number, author and other schematic information. This is beyond the
scope of this tutorial but more information can be found in the Templates chapter of
the accompanying reference manual (Help Menu – Schematic Capture Help).
Sometimes, it is desirable to have a base annotation for a sheet; this means that the global
annotator will increment from the value entered in this field. For example, if we set this to be 100
then the first resistor placed on the sheet would be annotated as R100. When left at its default
value the global annotation will continue from its current position – this is fine for the purposes
of the tutorial.
Setting initial annotation for sheets is useful as it can guide the Global Annotator
when batch annotating. It can - if you choose - also then be honored when
annotating physically via the Automatic Annotator in the PCB Layout Module.

38
Before exiting, your dialogue form should now look something like the following:
Edit Sheet properties with the Annotator set
For completeness we should also follow this process for the sheet we have just finished laying
out. Before we can change the properties of a sheet we must first navigate to that sheet in the
design and Proteus provides several ways to do this:
From the Design Menu select Root Sheet 2 at the bottom of the menu.
From the Design Menu, select the Goto Sheet command, select the sheet and click OK to
switch to that sheet.

Schematic Capture
39
Use the PGUP and PGDOWN keyboard shortcuts to navigate between sheets. These
cycle up and down the sheets respectively, although for a two sheet design they will
seem to have the same function!
The Design Explorer is also a powerful way to navigate the schematic – this is
covered in the Design Verification section of the tutorial and in more depth in the
reference manual.
Once you find yourself back on the sheet we have laid out simply repeat the process above,
with a sheet title of ‘MCU, sensors and memory’ and a sheet name of ‘1’.
Sheet 1 properties
You should now see correctly organized and labelled sheets at the bottom of the Design Menu

40
This is what you should see in the Design menu
Connectivity between Sheets
Now that we have taken care of the naming, let’s navigate back to our blank sheet and lay out
the analog circuitry. The following screenshot shows the circuit we need to draw.

Schematic Capture
41
As we can see, there are three logical blocks of circuitry; a reference generator for the ADC
module, an analog buffer for the pressure channel and a DC/DC converter to provide 5V from
the 3V battery to the other two sections on each pressure sampling time.
If you feel that you need more practice then you can use all of the techniques we have covered
so far to complete the schematic. Alternatively, if you are comfortable with the basics of
schematic entry we will load a pre-supplied completed schematic in the next section.
Regardless, there are a couple of points of note that are worth emphasizing.
Firstly, connectivity between sheets is achieved by having terminals with the same name on
both sheets. From the screenshot above you can see the named terminals and, switching to the
first sheet, the corresponding terminals with the same name. This technique allows signals to
propagate not only across a sheet but also across sheets.
Secondly, it is possible when placing wires to ‘guide’ the wire placement as you place the wire.
This is achieved by left clicking the mouse as you change direction, placing an ‘anchor’ to help
the follow-me algorithm place the wire the way you want. Typically, this is useful on more
complex wire trails but we can look at a simple example for the purposes of illustration.
Consider the connection between the negative input of U4:B and resistor R18 as shown here:
Negative input wire to R18
If we delete this wire (right click and select delete), we could replace the connection in the usual
way and the follow-me algorithm would make a decent job of it. However, if we wanted to be
more precise we could proceed as follows:
Hover the mouse over the negative input such that it turns green and then left click to
start wire placement.

42
Move the mouse along to the left and then left click the mouse once to place an ‘anchor’.
Move the mouse up, left click to place an anchor, then right, left click to place an ‘anchor’
and finally down onto the wire between the op-amp output and resistor.
This technique constrains the follow-me algorithm and provides greater control during wire
placement. If at any time during placement you change your mind and wish to remove an
anchor simple right click the mouse once. Finally, if you want to completely disable the wire-
auto-router and, for example, place a wire at 45 degrees, simply hold the CTRL button down on
your keyboard during placement.
Gateswap
Now that we have a multi-element placed (LM358 dual op-amp) it's a good time to look at gate-
swapping on the schematic. The reference for a multi-element part reflects both its part
reference (e.g. U4) and also its gate element identifier (e.g. A) as shown below.

Schematic Capture
43
U4:A and U4:B
Start by editing one of the LM358 gates (right click - edit properties) to bring up the Edit
component dialogue form.
Edit Component Dialogue form for an Op-Amp
To swap the gates we are switching the element identifiers (A and B) on a single part (U4). The
element field of the dialogue conveniently contains a combo box will all available gates so all we
need do is change the element and hit OK to commit.

44
On schematic this switches the gates over according to the change specified in Edit component.
Preparing for PCB Layout
Now that we have completed the circuit we need to give some thought to PCB Layout and the
information that we are going to provide from the schematic. A netlist basically consists of a set
of footprint names (packages associated with schematic components) and connections (wiring
on the schematic), although we can make things easier for ourselves later on by providing
additional information.
If you do not have a completed schematic at this point or wish to work with the pre-supplied
schematic you can load it via the Open Samples command on the Proteus home page. The file
name is dsPIC33_REC_SCHEMATIC.pdsprj.
Packaging Considerations
Ideally, each component in Proteus should be associated with a footprint in the PCB editor.
While you can do this at the point of placement in the PCB Layout, best practice would be to
sort this out in the schematic. Fortunately, the Proteus system provides a large set of pre-
packaged components where this work is all done for us. As a case in point, the schematic we
have just created requires no alteration or packaging work as the parts we have selected from
the libraries already have footprints assigned to them.
However, it is possible that you may want to change the footprint associated with a part (e.g.
PTH to SMT). We’ll use the current schematic as a playground to explore how we can view and
change packages to components.
To view the package associated with a component:
The footprint for a component is simply a property of the component in Proteus. We can
therefore easily view the footprint by editing the component. Try this now by right clicking on
one of the resistors on the schematic and selecting Edit Properties from the resulting context
menu. You should see that there is a PCB Package property on the dialogue form and that the
part is packaged with a standard 0805 footprint.

Schematic Capture
45
The new package appears in the Edit Component Dialogue form
You can also see what the default footprint is for a component at the time you
select it from the libraries. At the bottom of the Pick Devices dialogue form a
preview of the footprint is shown for the currently selected component.
For convenience, components in the schematic often have packagings for more than one
footprint. For example, if you launch the Edit Component dialogue form for the dsPIC33
component you will see that you have the option of either an SO18W or a DIL18 footprint. In this
case the designer can simply change the footprint if required via the Edit Component dialogue
form.
To change a package on a component
Launch the Edit Component dialogue form by right clicking on the resistor and selecting
Edit Properties from the resulting context menu.
Click on the question mark to the right of the package property to launch the footprint
browser

46
Clear out the text from the keywords field and then use the filters on the left hand side to
narrow down the selection. We will want to select the ‘Discrete Components’ category
with type ‘Through Hole’ and Sub-Category ‘Resistors’. We can then select for example
the ‘RES40’ footprint and click OK to commit.
You should now see that the RES40 is listed as the PCB Package for the component in
the schematic.
To change a package on all components of a particular type
If we want to make a wholesale change to parts already placed we can do so from the design
explorer. First, open the design explorer via the icon on the main toolbar and then switch to the
search tab:
Following on from our example above, let's set category to be Resistor and hit search

Schematic Capture
47
You should now see a filtered list of all the resistors on the schematic in a grid view. We could
filter further by entering a resistor value.
To change the package, simply type in the field at the top and then, much like Excel, drag the
value down the other entries in the column.

48
Hit Apply Changes to commit the change.
Some caution is required with bulk editing like this because the software will accept your
input without verification. It is however, extremely handy for changing passive footprints
en-masse.
Connectivity Considerations
When we transfer our schematic to the PCB Layout software (netlist) all of the wires and
connections are grouped into nets and passed through. Proteus actually does quite a lot of work
for us behind the scenes at this point, automatically generating numerical names for the nets
and also assigning the net to a default ‘net class’.
Net names are assigned by Proteus according to the following rules:
A group of connections which include a named terminal will be assigned a net name
according to the name of the terminal.
A group of connections which include an unnamed ground terminal will be assigned to
the GND net.
A group of connections which include an unnamed power terminal will be assigned to the
VCC net.
Any other group of connections is given an auto-generated numerical name.
What this means in practice is that all the work is done for us here; there is no real need for us
to get involved in naming groups of connections. It is important however, that we understand the
rules for unnamed ground and power terminals. If in any doubt, you should always name your
terminals explicitly.
If a net does not have a name from a terminal you can if you wish explicitly name a net by
placing a wire label with syntax (NET=NAME). This is useful if you wish to place a power plane
on the net in the PCB and otherwise helps to distinguish the net from other nets with auto-
generated names.
A ‘net class’ is simply a group of nets which will have common properties in the PCB Layout.
Specifically, all connections in a net class will have the same trace width and will obey a single
set of rules with regard to clearances and design rules. Again, Proteus will do a considerable
amount of work for us and will assign net classes as follows:
Any net with a power or ground terminal is assigned to the POWER net class.

Schematic Capture
49
Any net with a bus is assigned to the BUS net class.
Any other net is assigned to the SIGNAL net class.
This gives us quite a bit of flexibility during PCB layout as we can define different trace widths,
via styles, clearances and so on for each net class. Sometimes, however, we will need a
particular set of conditions for particular connections. Proteus allows us therefore to create our
own net classes and these will then be passed through to the PCB Layout software, allowing us
to define routing and clearance properties specifically for those connections.
Let’s take an example. On the tutorial schematic consider the output of the DC/DC converter on
the Analog sheet of our design. This is the 5V switched power supply for the analog circuitry so
we really want to lay this out with a track width smaller than that on the POWER net class but
larger than on the SIGNAL net class. The procedure for specifying a new net class is very
straightforward.
To specify a new net class
Select the Wire Label Icon.
Left click the mouse on a wire we wish to assign the net class to. Any wire on the net will
do – in our case let’s place it between the output of the MAX1724 and the SW_PW
terminal. You will see a small ‘x’ under the cursor when the mouse is over the wire.
Left click the mouse over the wire to launch the wire label dialogue form. Then simply
type in ‘CLASS=ANSW’ to assign the net class.

50
If you have completed drawing the schematic follow this procedure now to add the net class;
this will already be in place if you have loaded our pre-supplied schematic. If you work through
the PCB layout tutorial, you'll see how to configure routing styles and design rules for the net
class.
Design Verification
It is always a good idea to spend a little time checking the schematic before we move through to
PCB layout. Proteus provides a unique and extremely powerful tool in the form of the Design
Explorer that will help us catch any errors before we sign off on the schematic phase of design.
In this tutorial we will introduce the tool and cover some basic functionality but we do
recommend that you read the section in the reference manual (Help Menu – Schematic Capture
Help) and spend some time familiarizing yourself with its many capabilities.
Note that what you see in the Design Explorer throughout this section will depend
on whether you have drawn the schematic yourself or loaded the pre-supplied one
from disk.
The Design Explorer
The Design Explorer can be launched from top level application module toolbar and will appear
as a separate tab inside the Proteus application.
The Design Explorer icon
It is worth mentioning that, in terms of your Proteus workspace, you can detach tabs into
separate frames. This is particularly useful if you want to view more than one module at the
same time and have two monitors or a lot of space on screen. To split a tab onto its own frame
simply drag and drop it onto an area of free space. This will allow you to view both the Design
Explorer and the Schematic at the same time.

Schematic Capture
51
Split programs in Proteus
Alternatively, if you do prefer to work with tabs in a single frame you can quickly cycle between
tabs using the standard Windows CTRL+TAB keyboard shortcut.
Once launched and in its default mode, you should see a dialogue form that looks a little like
Windows™ Explorer. The left hand pane displays the sheets and the right hand pane displays
the contents of the currently selected sheet. Clicking on another sheet in the left hand pane will
force the right hand pane to show the contents of that sheet selected.

52
The Design Explorer
The Design Explorer has two distinct modes; partlist mode and netlist mode. The former will
show a physical representation of the sheets (the components on a sheet) whilst the latter will
show how the design is organized into groups of connections (nets). You can switch between
the two modes via the Design Explorer Icons.
Design Explorer icon bar
Since we are in partslist mode by default let’s look at what we can do from there. You may
remember that earlier in this topic we discussed how to check the packaging for a single part.
The Design Explorer shows us the bigger picture and allows us to make a global check of the
packagings on the design at a glance. All of the footprints used are displayed beside their
schematic reference at the far right hand side of the right hand pane so all we need to do is
scan down the list to make sure everything is packaged, switch sheets (via the left hand pane)
and repeat the process. If a part on the schematic did not have a footprint assigned it would
have bright red text stating 'MISSING' in this field to highlight the potential problem.
A quick scan will immediately show that we do not have a packaging associated with the LED
schematic part. Right click on the Design Explorer on the line with the LED and select Goto
Schematic Part from the context menu

Schematic Capture
53
The Design Explorer's context menu
This will zoom the schematic around the part and tag it for editing. Simply right click on the
highlighted part and select Edit Properties in the normal way. We could follow the procedure
that we discussed earlier to find a suitable footprint but in this case take it as a given that it is
named LED and simply type in LED in the PCB Package field of the dialogue form.
LED Assigned as the package
After making the change, the Design Explorer will live update to reflect the current status of the
schematic.
Design Explorer showing the LED packaged
Now, simply follow the same procedure as above to change the footprint to an 0805.

54
We can also use the Design Explorer to investigate the connectivity of the schematic – for this
we need to switch into netlist mode via the icon at the top left of the dialogue form. This will give
us a view as shown below.
The Netlist icon
The first point to note is the net names which, as we discussed earlier, are either named
according to terminal or label or simply assigned a number if the net consists only of wire
connections. We can right click on any net to view its connections on the current sheet by
selecting the ‘Goto Schematic Net’ option from the resulting context menu. This is particularly
useful when we want to check single pin nets for example, or if we want to name a net manually
(see the section on connectivity considerations earlier in the tutorial). Finally, where we have a
net or nets grouped with a named net class (far right column on the right hand pane) it can be
useful to check our assignments.
Goto Schematic Net will highlight the selected net
The Design Explorer is an extremely powerful tool and has many different uses
throughout the lifecycle of a typical project. In particular it can be used as a link
between the schematic and the PCB, facilitating cross-probing and PCB lookup. We
recommend that you read and work through the chapter in the reference manual
(Help Menu – Schematic Capture Help) for more information.
Assembly Variants
Assembly Variants provide a simple method of managing multiple product configurations in a
single schematic/pcb project. This is done by specifying the fitted or not fitted status of each
component on a per variant basis. They are often used for excluding parts from cheaper
versions of a product or for identifying PCB versions to firmware by controlling the use of pullup
resistors on an MCU port.
In Proteus, Assembly Variants are configured primarily through the Design Explorer. Let's look
at a simple example and we'll remove the SHT15 temperature and pressure sensor from a new

Schematic Capture
55
product variant. Start by creating the new variant from inside the Design Explorer and naming it
budget.
Notice that this gives us a new column in the component grid. Each entry currently has a tick
which indicates that the part is fitted on the board for the variant. If we click on the entries for the
budget column on U3 along with R5, R6 and R7 they will change to a cross. Clicking on the
apply changes button at the top will then set these parts to be excluded from the BUDGET
variant.
When you have more than one variant on the schematic you can switch between Active
Variants via the variant combo box at the top of the screen. When we switch to budget variant
you should see that the part reference for the temperature sensor circuitry will be greyed out to
indicate that the part is not present in the active variant.

56
We could also have done this by individually editing the parts and checking the exclude from
Active Variant box on the Edit component dialogue. You need to be very careful when working
this way to ensure that you have first selected the variant you want from the combo-box at the
top.
Finally, you can quickly manage variants for a group of parts by first dragging a selection box
around the parts and then showing selected in the search tab of the design explorer.
The Proteus software manages the variant information through all of the output systems,
changing the BOM Report, the Pick and Place files, the Assembly Drawings, the 3D Viewer and
any export for MCAD to reflect the fitted status of the parts. Assembly variants do not affect the
2D PCB layout.
You can add the @VARIANT text string to the schematic to indicate the current
variant on the schematic. This is a useful reminder and particularly important for
printing schematic documentation. See the header block in the schematic reference
manual for more information.
Bill of Materials
Constructing a Bill of Materials is an often necessary but frustrating task at the end of the
schematic design phase. Fortunately, Proteus provides a completely flexible scheme which
allows you to include as much or as little information as required.
Let’s start by looking at the default Bill of Materials Output. Launch the Bill of Materials module
from the application module toolbar at the top of Proteus.
Launch the Bill of Materials from the icon

Schematic Capture
57
The section at the top of the report is taken from the Design Properties Command, which you
can find on the Design Menu, and modify accordingly.
The Edit Design Properties dialogue form
If your Active Variant is not the base design then the Assembly Variant will also
be included in the header block:
Bill of Materials categories control the grouping of parts in the report and work by comparing the
reference prefix of the components. For example, all resistors have a prefix of ‘R’, capacitors a
prefix of ‘C’ and IC’s a prefix of ‘U’. Similarly, Bill of Materials Fields control the content of the
report with each field contributing a column.
Both fields and categories can be created, edited or deleted directly from the left hand control
panel on the BOM report.

58
Section for editing The Bill of Materials information
Let's work through a couple of examples. First, we'll order all our parts from Digikey so let's
specify a supplier in the BOM. To do this, we need a new field.

Schematic Capture
59
BOM Fields
Launch the BOM Field editor by clicking on the Add button underneath the Fields listing.
The 'Add' button enters the Edit BOM Fields dialogue form
If you are adding a field that you have previously defined then you select it from the drop down
combo box at the top of the dialogue form. However, since we have not defined a SUPPLIER
property before click on the new button to create a property definition.

60
Adding a New BOM field
There are two non-editable fields that you can apply namely .placed and .name.
The placed field will show whether the part is placed on the layout (component or
solder side) while the name field simply populates with the component names.
Property name is SUPPLIER, description can also be Supplier and Type is String.
New Property dialogue filled out correctly
We don't need to prefix or suffix values and this is not a numerical property so sub-totals are
meaningless. Click on the OK to exit the dialogue form and create the property.
At this point the BOM has switched to the Property Editor tab which is essentially a grid view of
the data in the report. We need to add information for each component in the Supplier column.
We could do this individually but since all of our parts are coming from a single supplier it's far

Schematic Capture
61
easier to use find/replace. Left click on the supplier column and then either use the CTRL+F
shortcut or click on the find/replace icon.
Find and Replace form
Leave the find edit box blank (we are entering data into blank fields), type Digikey in the
Replace edit box and make sure that the current column only checkbox is selected.
Replacing blank fields with 'DigiKey'
Hit the replace all button to enter the data. You should see that all of the fields in the Supplier
column are populated and coloured in blue.
DigiKey now appears where the blank fields were

62
The blue indicates that the changes have not yet been committed; if you have made a mistake
the clear pending changes button will revert your edits. When you have reviewed your changes
use the Apply Changes button at the top to commit.
Applying BOM Changes
If you switch back to the HTML View of the report you should now see the information you
entered in the report.
DigiKey is now assigned as the supplier
Also, if you return to the schematic and edit a component the data will be present there as well.
The Supplier field is automatically added in to the form
Changing the data in the edit component dialogue form will live update the BOM report.

Schematic Capture
63
The BOM updates live with any changes in the schematic
This process can of course be repeated as required with other properties such as RoHS, MoQ,
Lead Time, etc. More practical examples and detail can be found in the Bill of Materials
reference manual (accessed via the Help Menu in BOM Module).
Note that property changes are applied locally to the schematic components and
not to the library parts. If you want to update your parts with newly entered
information then run the 'Compile to Library' command from the Library menu. This
will put all components in the design (along with their new properties!) into a library
of your choice.
Having configured the information on the BOM you can generate the report from the export
options from the icons at the top.
Export options for the BOM
It is beyond the scope of this tutorial but you also have full control of the colour and styling of
the report. This works via the customize stylesheet button at the top of the HTML view and is
discussed in detail in the BOM Reference manual.
Printing
To print the schematic, first select the correct device to print to using the Printer Setup
command on the File menu. This activates the Windows common dialogue for printer device
selection and configuration. The details are thus dependent on your particular version of
Windows and your printer driver - consult Windows and printer driver documentation for details.
When you have selected the correct printer, close the dialogue form and select the Print option
on the File menu to print your design. There are a number of options available on this dialogue
form, all of which have context sensitive help and are also discussed in more detail in the
reference manual under Hard Copy Generation. For our purposes we will simply center the
schematic output on the page and print. Do this now by right clicking on the Print Preview and
selecting the Position Output at Center option as shown below.

64
You can also export the schematic directly in PDF format from the Output Menu (no driver
installation required).
The current schematic is now ready for board layout so if you have purchased a Proteus
PCB Design package you can move straight onto the accompanying tutorial booklet for PCB
Layout.
Library Parts
Introduction
The Proteus Design Suite comes with a significant installed base of schematic components,
almost all of which are already packaged with the correct PCB footprint. However, with the
number of new parts entering the market every day and the vast choice available to engineers it
is inevitable that users will have to either import library parts into Proteus or create library parts
inside Proteus.
Importing Library Parts
Importing Library Parts is by far the preferred option. It is both much faster to do, is far less error
prone and you can import both the schematic part and the layout footprint at the same time.
Proteus supports two ways to import parts:
Integrated Web Search and Import (Requires a valid USC)
Manual Library Part Import Dialogue.
Short tutorial videos on working with both methods can be found on our Youtube Channel

Schematic Capture
65
Web Search Import
The integrated web search import works directly from the library picker dialogue. You simply
type the part name you want and, after searching the installed libraries, you can search a
database of over 15 million parts from our partner Samacsys. This service requires a free
account to be registered with Samacys and a valid USC to import the parts.
Library Part Import Dialogue
This method enables you to manually import via the Import Part command on the Library
menu in either the schematic of the layout editors. This import will work with all major vendor
files such as those generated by Ultra-Librarian, Samacys, SnapEDA and PCB Library Expert
as well as through common supplier portals such as Digikey or RS Components. It does not
require a valid maintenance contract to work but does involve slightly more effort.

66
The Import Part dialogue with a part loaded.
Technically, the import works with PADS Library V9.x files, meaning that the import will work
with any supplier who can generate a fileset in this format.
To import a library part using the library picker
Web search import works as follows:
1) Launch the library picker in the schematic module (also 'P' on the keyboard).
2) Search for a part. If matches exist in the installed libraries they will be shown
and you can click to open web search results from the bar at the bottom of the picker.
If there are no matches from the installed libraries you will go directly to web
search results.

Schematic Capture
67
3) Results in normal font are available for import. Results in disabled text can
be requested (at no charge) from the build service form.
4) Double click to import. The first time you do this you will need to supply credentials
or create a free account.

68
5) When you double click to import, both the schematic part and the associated PCB
footprint will be brought into your user libraries and also picked into the current
project. In most cases, the 3D STEP file for the footprint will also be imported.
If you need to request a part to be made you can do so directly from the pick dialogue
by double clicking on one of the disabled entries in the web search. The service
is free of charge and average turnaround is 24-48 hours.

Schematic Capture
69
Import Library Part using the Dialogue
1) Download the part you want onto your computer. This will almost always be in a zip file.
2) If the part doesn't come from a vendor source that we directly support (see here) then you'll
need to extract all the files from the zip into a folder of your choice.
3) From the Library Menu in Proteus select the Import Part command.
4) Click on Select File and use the file selector on the right hand side to select either generic
PADS Library V9 files or the vendor of your choice.
5) Choose the appropriate file to load. This will normally be a zip file if the vendor is selectable
in the file selector or a .p file if you've had to extract the parts into a folder.

70
6) Review the parse log and the previews to make sure everything looks good. Use
configuration settings if need be to fix problems.
7) Use Import Part and follow the wizards to bring first the footprint and then the component into
Proteus. This will both put the parts into your libraries and deposit them in the parts bin of the
current project ready for placement. You should have an end parsed result that looks like the
following:
What you are actually doing at this last stage is running the Make Package tool to create the
footprint and then running the Make Device tool to make the schematic component. The areas
where input may be required from you are in the library choice and the description and
categorization of the part.
For most complex devices, you can also find a BSDL script from the manufacturer. This is
schematic part only but can be imported via the same import part command (select BSDL in
stage 4 above).
Creating New Devices
If all else fails you can create parts yourself entirely inside Proteus. Alternatively, you may wish
to permanently adjust the properties or footprints of an existing component. This section of the
documentation starts from the basics of creating a new device and covers the entire process
through to storing the new part in the library.

Schematic Capture
71
While the following topics are a detailed explanation of how to create component parts in
Proteus, in practice this should almost never be necessary. In addition to the many installed
libraries Proteus includes a web search with access to 15 million library parts and also the
universal part importer provides support for almost all third party part vendors (Ultra-Librarian,
Samacsys, SnapEDA, etc.). If the part doesn't exist in Proteus itself the next step is to search
for and then import it directly from a third party vendor. This is discussed in some detail in the
importer help file and shown on our Youtube Channel.
Graphics and Pins
For our example part let’s assume that we want to create a Microchip MCP23008 I2C expander.
The first thing we need to do is to create a graphical representation of the part on the
schematic. When we are finished it should look something like the following:
The MCP23008 Completed
Let’s begin by placing the component body as follows:
Select the 2D Graphics Square icon and make sure the component style is selected in
the Object Selector.

72
Left click once on an empty area of the schematic to begin placement.
Move the mouse until the rectangle is around the size of the part that you want. It’s better
to make this slightly larger than might be required as we can easily resize it later.
Left click again to complete placement of the graphic.

Schematic Capture
73
Proteus supports a powerful graphics style system of local and global styles and the
ability of local styles to follow or track global styles that allows you to easily and flexibly
customize the appearance of your schematic. See the section Graphics and Text Styles
in the online reference manual for a complete explanation of how styles work and how
they are used.
The next job is to place the component pins.
Select Component pin mode and make sure that you have the default pin type selected in the
Object Selector.
1. Left click the mouse on the schematic to begin placement. The small cross at the end of
the pin indicates the side of the pin that will be wired to so it is important that this is
outward facing.
2. Move the mouse so that the other end of the pin touches the edge of the component
graphic and left click again to place

74
3. A new pin is automatically primed for placement so simply move the mouse down slightly
and left click to place again.
4. Repeat the process down the left hand side of the component graphic using the
completed screenshot as a reference. Right click to finish placement.
5. Click on the X-Mirror icon to point the pin in the opposite direction ready for placement
down the right hand side.
6. Repeat as of stage 3 to place the pins down the right hand side of the component.
7. Right click the mouse when you are finished to exit pin placement mode.
The Plus (+) and Minus (-) keys can also rotate the pin during placement, but you will find
that when adding pin numbers, they will be on the opposite side of the pins that you placed
before rotation. In this case right click on the pin(s) affected and click the Y-Mirror option to
correct the pin(s).

Schematic Capture
75
At this stage your component graphics should look something like the following:
The body of the MCP23008
The actual positioning of the pins is of course somewhat aesthetic and you may prefer to have
different groupings to those we have chosen.
Now that we’ve placed the pins we may need to adjust the size of the component body. If you
need to adjust the size of the component body to better fit. To do this, click on the Selection
Mode icon and simply left click on the edge of the component body, then left depress the mouse
on one of the nodes, drag to the new size and release the mouse to commit.
This works much like any other graphics package. For example, if you right click along the
bottom you can drag up and down and if you right click on an edge and you can drag
diagonally. Make sure however, that you do not leave any of the pins ‘hanging’ (not touching)
when you do this, else you will have to subsequently move the pins back onto the component
edge.
If you want to make fine adjustments you may need to adjust the Snap level – these options
are available from the View menu in Proteus (defaulted to 0.1in) and are discussed in more
detail in the reference manual.
Now that we have the basic shape of the part we need to add names to the pins. This can be
done as follows:
Right click on the pin at the top left of the component and select Edit Properties from the
resulting context menu.

76
Type in the name of the pin (SCL), the default pin number (1) and the electrical type
(INPUT). You can use the other options to control visibility but for our purposes the
defaults are fine.
Hit the Next button at the bottom to switch to the next pin in the list and repeat the
process – the schematic will update to show which pin you are editing. If you are
unfamiliar with this part and don’t therefore know the electrical type of the pin simply
leave it as the default Passive type.
When you get to the RESET pin you’ll need to add an overbar. Do this simply by adding a
dollar (‘$’) prefix and suffix to the name.

Schematic Capture
77
Hit the OK button when you are finished.
You may have noticed that there is a significant omission from the schematic part as we have
drawn it so far, namely that there are no physical power pins on the device. Since we do not
need to wire power nets explicitly we do not need a physical pin for the component. We need
only ensure that the power pins are handled correctly with respect to the physical PCB footprint
and we’ll discuss this in more detail in the next section. It is worth noting however, that while it is
very common to have non-physical power pins in order to reduce clutter on the schematic, you
may have a preference for everything to be explicitly wired. In this case you could simply add
two extra pins and name them VDD and VSS respectively.
Our final task now is to make a device from the composite graphics and pins that we have
placed. Start by drawing a tag box around the entire graphic (right depress the mouse and drag
the selection box). Next, right click the mouse inside the selection box and select the Make
Device option from the resulting context menu.

78
Make Device icon and the Context menu option
This presents us with the Make Device dialogue form, where we can customize the part. All
fields throughout this wizard have context sensitive help associated with them, accessed by
clicking on the question at the top right and then on the field in question. However, the only
items we need to deal with here are the Device Name and the Reference Prefix. The device
name should be MCP23008 and the reference prefix should be ‘U’.
The reference prefix serves to categorize parts for Bill of Materials Output and is
also used in annotation. These are fairly standard across the industry with ‘R’
denoting resistors, ‘C’ for capacitors, ‘U’ for IC’s and so on.
Use the Next button at the bottom of the dialogue to move onto the next screen.
Adding Footprints
In a previous section of the documentation we saw how to quickly add a footprint to a schematic
part. This is useful for small passives and simple parts but, when we are creating a device we
need to follow a more complete procedure. This ensures not only that we have a correct

Schematic Capture
79
mapping between the pins on the component and the pads on the footprint but also allows us to
better handle power pins.
From the screen on the Make Device dialogue form click on the Add/Edit button to launch the
Visual Packaging Tool. The first thing we need to do is to find the footprint we want to use so
click on the Add button at the top of the dialogue form.
The 'Add' button in the Packaging Tool
This brings up the package browser dialogue which we covered earlier in the documentation.
Assuming that we want the surface mount package, type SOP18 in the Keywords field and then
double click on the part in the results list to select it.
Selecting the SO18W from the package library
The Visual Packaging Tool will now look something like the following screenshot.

80
There are several points of note here. Firstly, the pads in the preview which are white are
deemed to be mapped onto component pins. This has happened as we have correctly specified
the default pin numbers when we edited the pins earlier on (pad name maps onto pin number
when present). If we had chosen to leave the pin number fields blank we would have to map all
of the pins in this dialogue form.
Secondly, we can see that there are three pads (7, 9 and 18) which are not mapped onto
component pins. Normally we would have the datasheet beside us to get the footprint mappings
but in this case pin 7 is an NC pin, pin 9 is the VSS pin and pin 18 is the VDD pin.
The NC pin is easily handled – simply type 7 in the field for NC Pins. Notice that the preview on
the right hand side will update to show that this pad is now considered dealt with.
We now need to add two ‘virtual’ pins for the power pins. These are pins which don’t need to be
on the schematic (their connection is made implicitly according to their name) as they will add
unnecessary clutter, but do need to be mapped onto pads in the footprint.
If you want to have all pins visible on the schematic (e.g. for auditing purposes) you
can certainly do so. You would add another three pins to the device, connect one of
them to an NC terminal (to put on the NC net) and connect the other two to power

Schematic Capture
81
terminals with the correct names. If you are in any doubt regarding power nets and
connections please see the section earlier in the document on powering the circuit
or consult the reference manual.
Click on the Add Pin button underneath the grid, type VSS to name the pin and then repeat the
process for the VDD pin. Remember that connections to these virtual pins are made according
to their name so make sure that you name them correctly.
Adding a virtual pin
Having created the pins we assign them to pads on the footprint as follows:
Click in the column at the far right of the VSS pin.
Click on the corresponding pad on the footprint (pad 9).
The cursor will move down to the next pin (VDD) so all we need to do is click on pad 18
on the preview.
Clicking on pads will assign the pin

82
We should see that all the pads on the footprint are now highlighted, indicated that the part is
fully packaged. Simply hit the ‘Assign Package’ button at the bottom of the Visual Packaging
Tool to commit and return to the Make Device dialogue form.
It is possible (and extremely useful) to have more than one packaging for a given
component. We could, for example, follow the exact same procedure to add a
DIL18 footprint to the component. Where more than one packaging exists you can
specify the one which will be used by default by checking the default box
underneath the package name in the Visual Packaging Tool.
Click the next button at the bottom of the dialogue form to move onto the Property definitions
section.
Adding Properties
This screen allows us to add component properties to the device. We looked at doing this on a
particular instance of a device (the part on the schematic) earlier in the documentation; the
difference is that properties entered here will be stored in the master library part and therefore
available every time we use the part in a design.
We can see that the PACKAGE property is already defined – this was what we configured
visually on the previous screen
Package preview on the Make Device form

Schematic Capture
83
Let’s assume we want to add a property for RoHS compliance.
Start by clicking on the New button at the bottom left and then clicking on Blank Item.
On the right hand side fill out the name as ‘ROHS’ and the description as ‘RoHS
Compliant’
The next field is the data type which in our case is a simple Boolean (Yes/No) – select
this from the drop down list.
Change the Default value to be Yes and leave the visibility defaults as they are.
If you want to add more properties (e.g. MoQ, Price, Code, Supplier, etc.) simply repeat the
process above. Alternatively, the Bill of Materials provides a convenient way to apply data to
schematics as discussed earlier in the tutorial. Finally, for complete control or if you are doing
this on a large scale, we recommend you read up on ASCII Data Import in the reference
manual.
Click the next button at the bottom of the dialogue when you are finished to move on to the next
screen.

84
Attaching a Datasheet
This screen allows us to attach a datasheet to the part we are creating. To do this we would
need to enter the filename for the datasheet and then configure the path as required. As we
don’t have a datasheet handy we’ll ignore this step but the following screenshot shows an
example of how we would set it up.
Adding a datasheet to the component
The main advantage of working through this step is to have the datasheet handy when you
place the part. If present, you can simply edit the component and click on the Data button at the
right hand side.
The Data button will launch the assigned Datasheet
For convenience, we have configured many of our library parts with datasheets
which you can download from our web server via this button.

Schematic Capture
85
Indexing and Library Selection
The final screen allows us to categorize our part and choose which library we will place it in. As
we have seen earlier in the tutorial the part description and the categories are used as filters
when finding and selecting parts from the library so it is worth giving some thought to your
description. An example of what you might enter is shown in the following screenshot.
Final section where you save the component to a library
When you are finished simply click the OK button. You will be prompted to replace all instances
of the device on the schematic – this allows you to update the current design if you are
modifying a part which already exists on the schematic.
Finally, if you now select the part from the Object Selector and edit its properties you should see
something like the following screenshot.

86
Edit Component for the MCP23008
It is also possible to create multi-element parts in Proteus. While beyond the scope
of this tutorial these are covered in the reference manual.

87
PCB LAYOUT TUTORIAL
Introduction
The purpose of this tutorial is to familiarize you as quickly as possible with the main features of
the PCB Layout, to the point that you can use the package for real work. Users with modest
computer literacy should find it possible to learn the package and produce their first board within
a day or two.
The tutorial proceeds by taking you through worked examples involving all the important
aspects of the package including:
Basic techniques for placement and routing.
3D Board Visualisation.
Netlist based design including both manual and automatic routing.
More advanced editing techniques such as block editing and route editing.
Report generation.
Hard copy generation.
Library part creation.
We do urge you to work right the way through the tutorial exercises as many things are pointed
out that if missed will result in much wasted time in the long run. Also, having worked through
the tutorial and thus got a basic grasp of the concepts behind the package you will find it much
easier to absorb the material presented in the reference chapters.
Note that throughout this tutorial (and the documentation as a whole) reference is
made to keyboard shortcuts as a method of executing specific commands. The
shortcuts specified are the default or system keyboard accelerators as provided
when the software is shipped to you. Please be aware that if you have configured
your own keyboard accelerators the shortcuts mentioned may not be valid. You can
configure your own keyboard shortcuts via the System - Set Keyboard Mapping
command.
Menus toolbars and icons all switch when you change between tabs to reflect the
functionality of the module you are working on. When we talk about menu
commands or icons in this tutorial we assume that the PCB layout tab is selected.
The menu contents will be very different if the schematic tab is selected!
Overview of the Layout Editor
We shall assume at this point that you have installed the package, and that the current directory
is some convenient work area on your hard disk. This tutorial is a direct continuation of project
we started in the schematic capture tutorial so we will start by loading the project file with the
completed schematic.

88
From the home page in Proteus click on the Open Sample button, filter to the tutorials category
and then select the dsPIC33 Recorder (schematic only) sample.
Opening a Tutorial sample design
This will open the tutorial project with the completed schematic from the Schematic Capture
tutorial. We can start the PCB layout module from the application module toolbar at the top of
the Proteus application.
If you are working on two monitors or have free screen space you can drag and
drop one of the tabs to view both modules simultaneously. If not, you can switch
between the tabs with the mouse or via the standard windows CTRL+TAB shortcut
key.
Much of the look and feel of the application is similar to Proteus and hopefully now familiar,
although there are some important differences.
The Main Window
The largest area of the screen is called the Editing Window, and it acts as a window on the
drawing - this is where you will place and track the board. The smaller area at the top left of the
screen is called the Overview Window. In normal use the Overview Window displays, as its
name suggests, an overview of the entire drawing - the blue box shows the edge of the current
sheet and the green box the area of the sheet currently displayed in the Editing Window.

PCB Layout
89
However, when a new object is selected from the Object Selector the Overview Window is used
to preview the selected object – this is discussed later.
PCB Layout Window
The Control Bar
The control bar at the bottom of the application is different from what we have seen in the
Proteus application and essentially splits into five sections:

90
At the left hand side is the Selection Filter which allows you to configure both the layers and the
objects that will be selected in the current operating mode. Typically, the default rules will suffice
and this serves simply as a convenient override where you may wish finer granularity in
selection at a given time. The Layer Selector combo box also determines the current layer or
layer set and also applies to the placement of PCB objects.
The Layer and Selection filter
In the middle is the Status Bar which provides textual ‘hints’ on the object currently under the
mouse. This is particularly useful when you hover a mouse over a pad for example, as it will
inform you which net the pad is on.
The Status bar shows what the mouse is pointing at
Next, we have the connectivity status which controls the syncing of the PCB to the schematic
and - when everything is synchronized - doubles as a live connectivity checker.
Netlist Information and CRC information on the status bar
Next to the connectivity status is the live Design Rule Checker. This will report any physical
design rule violations that occur while the board is being designed. A left click on this will launch
a dialogue detailing the violations with the further option of zooming in to examine a particular
error.
DRC information on the status bar
Finally, at the far right hand side is the co-ordinate display which reads out the position of the
cursor when appropriate. These reflect not the exact position of the pointer but the location to
which it has been snapped. Default snapping options are selectable from the View menu (or via
keys CTRL-F1 and F2 -F4) and the snap values can be configured from the Grids command on
the Technology menu
Mouse Co-ordinates

PCB Layout
91
The co-ordinates can be in imperial or metric units as set by the Metric (default key mapping 'M')
command. You can also set a false origin using the Origin command (default key mapping 'O')
in which case the co-ordinates change colour from black to magenta.
The dot grid on the Editing Window can be toggled on and off using the Grid command, or via
its keyboard shortcut (by default this is ‘G’). The spacing of the dots normally reflects the current
snap setting, except when zoomed out. In this case, the dot spacing is set to a suitable multiple
of the snap spacing.
The PCB Layout can be set to display an X cursor at the position to which it has snapped the
pointer through the X-Cursor command, default key mapping is 'X'.
We’ll become familiar with all of these items and use them regularly as we work through
placement and routing of the board.
Navigation
Navigation of the layout (middle mouse zoom, panning, keyboard shortcuts, etc.), is identical to
the Proteus schematic capture package. Refer to the Proteus Getting Started Guide or the
Proteus reference manual for more information.
Visual Aids to Design
The PCB Layout package will use visual effects to help you understand what is happening
during board layout. There are two principle techniques:
Proteus will ‘twitch’ an object when that object is under the mouse and the selection filter
enables selection of that object type. This serves to identify when an object is ‘hot’.
Proteus provides dynamic cursors which change to identify what a left click will do at any given
time (place an object, select an object, move an object, etc.). A list of cursor types is shown
below.
Cursor Description
Standard Cursor
Placement Cursor - Left click will place and object according to mode.
Selection Cursor - left click will select the object under the mouse.
Movement Cursor - left drag will move the object selected.
Throughout this tutorial – and indeed whenever you are working in the Layout module – you
should make use of these visual indicators to as an aid to understanding the software.
Proteus 8 includes a multi-level ‘undo’ and ‘redo’ system via the shortcut keys
CTRL+Z and CTRL+Y respectively. If you make mistakes throughout the tutorial
remember that you can unwind as many times as you need to!

92
Display Options
Proteus is capable of harnessing the power of your computers graphics card to speed up
operation and provide true layer transparency on the layout. However, as not all machines have
sufficient graphics cards the software is also capable of using Windows to perform display and
graphical operations. The three modes of operation are called:
Windows GDI Mode.
OpenGL Hardware Accelerated Mode.
Direct2D Hardware Accelerated Mode
Proteus will test your computer when you first open the application and, if possible, will then set
a default hardware accelerated mode for you. Control over hardware acceleration and display
options can be found via the Set Display Options command on the System Menu. Some options
are relevant only to a particular mode and will be disabled if you select a different mode.
Graphics Mode
The first section of the dialogue reports on whether your graphics card will support OpenGL or
Direct2D hardware acceleration and, if so, allows you to switch from Windows GDI mode into
one of these two modes.
Select the best option that your graphics card supports.
Opacity
When a hardware accelerated display mode is selected the Opacity section of the dialogue
allows you to configure the transparency of various layers on the board.
Opacity options

PCB Layout
93
When using hardware acceleration, Proteus places special significance on the current layer,
giving it a higher opacity than other copper layers on the layout. This means that objects on the
layer you are working are clearly visible and that objects on the other layers of the board are
dimmed. You can control the relative opacity of both the current layer and the background
layer(s) using the sliders on this section of the dialogue form. For example, if you wish to
disable transparency altogether you could set the background layer slider to maximum.
Additionally, with hardware acceleration you can live view the solder resist and paste mask
around pads and vias on the layout (turn on/off from View Menu - Layers). When enabled, you
can also adjust the opacity of these layers using the appropriate slider controls
If you are working on complex, multi-layer PCB's it can be useful to define a number
of preset views for the board. This is done by creating new colour sets in the
displayed layers dialogue (e.g. TOP_VIEW, BOT_VIEW) with appropriate layers
visible and assigning them keyboard shortcuts.
Auto-Pan Animation
In Proteus, holding down the shift key and bumping the mouse against the edge of the Editing
Window allows you to pan the screen. Similarly, dragging an object against the edge of the
Editing Window will pan the screen in the direction of the drag. This navigation feature is called
auto-pan and is controlled via the options in this section of the dialogue form.
Auto-Pan options.
You can adjust the distance moved on auto-pan (pan distance), the number of steps taken to
cover this distance (number of steps) and the speed of the animation (pan time). These options
are available regardless of which mode of operation you have specified.
Highlight Animation
When working in hardware accelerated mode objects under the mouse with smoothly increase
their intensity to inform you that they are selectable. The highlight animation options in this
dialogue allows you to control the smoothness and speed of this effect.
Animation Speed options

94
The animation interval controls the frame rate of the animation and therefore the smoothness of
the fade-in/fade-out effect. Normally, the default value for this is suitable.
The attack rate specifies the speed at which an object will go from ‘fully off’ to ‘fully on’ whilst the
release rate allows you to adjust the speed at which an object will return from ‘fully on’ to ‘fully
off’.
These options are only available in hardware accelerated modes.
Multi-Sampling (Anti-Aliasing)
Multi-Sampling is a method used by graphics cards to reduce anti-aliasing effects when
graphics are displayed at different zoom levels. It is particularly applicable to text but impacts on
all graphics on the layout.
When working in OpenGL mode you can specify the level of multi-sampling you want to use.
The higher the level of multi-sampling the better the resulting display but the more GPU
resources are consumed. If you select a level of multi-sampling which is not supported by your
graphics hardware the software will reset the level to the closest one which your card can
handle. For normal operation in Proteus a multi-sampling level of 4x is quite sufficient.
Displayed Layers Dialogue
The displayed layers dialogue allows you to control the visibility and colour of the various layers
on the board. You can launch this from the View menu in Proteus or by clicking the mouse on
the status bar at the bottom of the application.
You can change the colour of a layer by clicking on the colour beside the layer and control the
visibility of the layer via the checkbox beside the layer (where appropriate). All changes are
updated live on the layout.
You can switch between the pre-supplied colour profiles (print and screen), create your own
colour profiles via the 'new' button at the top of the dialogue form and assign them to keyboard
shortcuts. This allows you for example to have a TOP colourset showing only top copper, top
silk, top resist and top paste mask. More information is available via the context sensitive help
for the dialogue form (click on the question mark at the top right of a dialogue and then on a
field of the dialogue form to launch).

PCB Layout
95
Finally, if you are working in OpenGL or Direct2D mode, the Resist/Paste Mask Display options
allow you turn on full display of these layers on the board, showing the resist and paste
coverage around pads and vias. When enabled you can change the intensity of these layers by
switching to the Thru-View settings tab and adjusting the appropriate slider controls.

96
Component Placement
Proteus 8 works with a live netlist so the PCB Layout module already has much of the
information we need to start the layout process. In particular, we have specified which footprints
are associated with each schematic symbol and Layout module can therefore pre-select these
for us ready for placement. This brings us to an important distinction in the software; the
difference between a component and a package.
Components and Packages
A component is an instance of a footprint that has been netlisted through from the
schematic.
A package is a physical footprint that exists in the PCB Libraries.
Selecting component mode will access footprints which have been specified as relating to parts
in Proteus and carry connectivity information whereas selecting package mode will access
‘unbound’ physical instances of a footprint. When working with a layout which is driven from a
schematic we therefore exclusively use component mode.
The Component Mode icon is second from the top directly underneath the Selection icon.
Clicking on this will display a list of items in the Object Selector which correspond directly to the
parts in Proteus that we used to create the schematic.
Component Mode
The Package Mode icon is directly underneath the Component mode icon and clicking on this
will show us the physical footprints corresponding to the components in the layout.

PCB Layout
97
Package Mode
When placing, routing and laying out a PCB based on a schematic (such as with this project) we
will be working with components.
The Board Edge
Before we can place the components on the board we need to define what shape and size the
board will be. For our project we need only a simple rectangular board edge but we do want to
control the dimensions of the board (115mm wide and 40mm high).
The first thing to point out here is that Proteus will operate in either imperial or metric units and
you can switch between modes either by toggling the Metric command on the View menu or via
the ‘M’ keyboard shortcut. You may need to switch units for the placement of the board edge
and also elsewhere in the documentation.
You can set your default or preferred units from Technology Menu - Grid
Configuration command.
To start placing the board edge, select the 2D Rectangle icon from the left hand side of the
application.

98
2D Box Icon
Next, change the Layer Selector to the Board Edge Layer.
Board Edge layer selected
Move the mouse to the approximate starting point (e.g. top left) for the board edge. Now, hold
the mouse still and press the ‘O’ key on the keyboard to set the origin of the co-ordinate system
to the point under the mouse. This will be reflected in the co-ordinate display at the bottom right
of the application. Left click to start placement and drag in the normal way. The co-ordinate
display at the bottom will show you the dimensions of the board edge as you drag.
Drawing a board edge
Press the ‘M’ key on the keyboard to toggle between metric and imperial units as required.
Once you have the desired size of board edge click left again to commit placement. Don’t worry
about where in the Editing Window you have placed the board edge – we will move it to the
centre of the world area shortly.

PCB Layout
99
Placed board edge which is always Yellow
If you would like the board edge to be a specific size, edit the board edge graphic
and set the dimensions to your requirements:
Finally, restore the co-ordinate system to its global origin by pressing the ‘O’ button on the
keyboard again. The colour of the co-ordinates will change from Magenta to black to indicate
that the global origin is now in use.
Co-ordinates at 0,0
Placing a board edge should always be the first task as the software needs to know
the boundaries of the board in order for example, to know the limits of where the
autorouter can function or the size of a power plane.
If you need to delete the board edge or resize it you can do so via the context menu options and
drag handles that will appear when you right click over the board edge graphic.

100
Select Delete from the context menu
Complex board edges can be directly imported onto the board edge layer using the
Import DXF function on the File Menu.
Layer Stackup and Drill Spans
Before we begin layout, we need to define our layer stackup and specify which drill ranges are
valid for vias. Start by launching the layer stackup dialogue from the Technology menu.
We will be making a simple two-layer board with a single core between top copper and bottom
copper. This will be shown visually on the editable grid and as a cross section in the board view
tab.
Since the defaults are fine for us, there is no action required here. If we did want to edit the
stackup then we would do so via the stackup wizard button which would allow us to change the
number of copper layers and the construction method for the board.

PCB Layout
101
Similarly, on the drill spans tab there are no additions required, since our target PCB is 2-layer
only. However, to provide some context to the topic, the following are some screenshots from a
6-layer stackup.
The most important thing to remember is that for multi-layer boards, configuration of this
dialogue is really important. We'd encourage you to read through the dialogue level help and if
you are unsure about anything, the topic is discussed in detail in the reference manual.

102
Work Area, Co-ordinates and Snap
It is likely that your board edge covers a small portion of the Editing Window, which is less than
ideal as all of the work will be taking place inside this area. We can of course zoom into the area
(point the mouse and roll the middle mouse button or use the F6 key) but the default zoom level
is designed to show the entire Work area. The Work area is the area inside the dark blue box at
the edges of the Editing Window. Let’s tidy this up a bit before we move on.
Start by switching into Selection Mode and then left click and drag a selection box around the
board edge.
Selection mode and the board edge selected
If you get it wrong and don’t completely cover the board edge, use the green handles to resize
the selection box until it completely encompasses the board edge.
Resizing a box by the drag handles
Now place the mouse inside the selection box, depress the left mouse button and drag into the
centre of the work area, releasing the mouse button to commit the placement.
Moving the board edge

PCB Layout
103
This is a very important technique worth mastering as it allows you to easily block
select and then perform actions on (move, delete, etc.) groups of objects.
Having centered our board edge in the Work area we can shrink the work area to a suitable
size. From the Technology Menu, select the Board Properties command and then set to
something like 175mm by 100mm, such that the resulting work area forms a reasonably
boundary to the board.
Setting the board properties
We saw briefly when placing the board edge that we can specify a temporary origin and use
that to place items of a given size (or to place items a specific distance away from our origin
point for example). We can however, also specify the location of the Output Origin. This is the
default origin used whenever we do not explicitly set a temporary origin and is shown on the
layout as a small blue marker.
It can be useful to move this to a corner of the board and particularly so if we have mechanical
constraints that we need to consider during placement (e.g. mounting hole locations). For our
design, we’ll move the origin to the bottom left corner of the board edge.
1) From the Output menu choose the Set Output Origin command.

104
2) Move the mouse towards the bottom left of the board edge. Roll the middle mouse button as
required to zoom in for more accurate placement.
3) Left click the mouse to commit placement.
The co-ordinate display will now provide values relative to the position at the bottom left of the
board by default, and relative to any specified temporary origin when set.
Remember that you can also toggle metric or imperial units via the command on the
View menu or the ‘M’ keyboard shortcut.

PCB Layout
105
A useful trick once we have specified our origin is to use the Goto-XY command on
the View Menu to move the mouse to the exact location we want to place position
sensitive parts. This command will automatically switch between X-Y or Radius-
Theta depending on whether you are in polar or cartesian co-ordinates.
Proteus has a default grid and will snap objects onto the grid, making it easy to form
connections and control board layout. There are four hotkeyed snap settings for both metric and
imperial units, changeable from the View Menu or by keyboard shortcuts. It follows that
changing the snap setting to a lower unit will allow finer granularity, whereas raising the snap
setting will make it easier to select objects at higher zoom levels. It is not advisable to change
the snap settings regularly through a design but rather to choose the highest appropriate setting
for the board you are working on.
You can change the four default snap settings via the Grids command on the Technology Menu.
Grid settings can be set according to the users requirement
The grid display itself can be toggled between off, dots and lines via the ‘G’ key on your
keyboard, whilst the colour of the grid can be configured from the Displayed Layers Dialogue
(View Menu).
Placing Components and the Ratsnest
Now that we’ve handled all the basics we can finally start to get our components on the board.
The following screenshot shows a fully placed board and we can use this to get our
approximate positioning. Since it is a fairly simple board we are going to place manually but it is
worth noting that Proteus includes a fairly sophisticated auto-placement facility that includes
component grouping (e.g. powersupply, usbengine, etc.) and floorplanning on the layout.

106
dsPIC33 board un-routed
Placing a component in the Layout is very similar to that in the schematic.
Start by selecting Component Mode from the left hand side icon set and then ensure that the
layer selector is set to Component Side – we won’t be placing any solder side components in
this project.
Component mode and the Layer Selector
The object selector by default will contain a list of all parts to be placed. For more complex
boards however it is worth noting that you can restrict the display to only items selected on the
schematic or only those on the currently selected schematic sheet.

PCB Layout
107
Components selected in Proteus and shown in the Layout - Component 'tagged' mode
This allows you to select parts of your design in the schematic and then work on placement and
routing of them in PCB Layout without the clutter of other components in the object selector.
Our layout however is relatively simple so we will work globally (all of the components available
in the object selector).
Let’s get the AA battery holder down first on the right hand side of the board. Select J1 from the
Object Selector, position the part using the previous screenshot as a guide and then left click
again to commit placement. Note that once we have placed the part it is removed from the
Object Selector and we can continue by placing the J2 connector above and towards the right of
the battery.
You should notice both during placement and afterwards that there are green ‘elastic’ lines
between the two components and also a yellow arrow from each component. The green lines
are ratsnest lines and indicate connections that have to be made between the two parts, whilst
the yellow arrows (named ‘force vectors’) indicate a preferred position for the part to minimize
ratsnest distance. The force vectors are provided as guidance only and are based solely on
logic to reduce ratsnest lines. Since we will be using the earlier screenshot to dictate positioning
we can turn them off.

108
dsPIC33 board as you see it having placed all the components
From the View Menu, select the Edit Layer Colours/Visibility command. The resulting dialogue
form shows all the layers in the layout with colour and visibility configuration options. All we
need do here is deselect the checkbox for the ‘Vectors and Ratsnest’ layer and exit the
dialogue.
The Ratsnest and Force Vector layers turned off
You can also launch this dialogue form by clicking the mouse on the status
reporting bar at the bottom of the application.
It is important to remember that this dialogue form controls visibility only; to control
whether objects on a layer were selectable/editable we would use the Selection
Filter which is discussed in more detail later in the documentation

PCB Layout
109
You may find that you need more control over the positioning in order to move connector J2 into
position. Remember that objects are linked to a snap grid so all we need do is reduce the snap
grid via the options on the View Menu, for example to 1mm snap.
If you are working in imperial units you can either change the snap to 25th or use the ‘M’
shortcut to switch to metric units
Now that we have the granularity we need, simply right click on the part to select it and then
drag it into the desired position. We can move the connector closer to the board edge if we
move the part label underneath the part. Again, the process is identical to the one we covered in
the Proteus tutorial – remember this time to right click on the label itself and not the component
body.
As you place components and ratsnest lines appear the connectivity status also will update to
show the number of missing connections.

110
J1 and J2 placed with the CRC showing 1 connection missing
A missing connection is essentially a wire connection on the schematic that has not been routed
on the layout. It follows that when the board is completed the connectivity status should report
no missings. We'll look at this is more detail when we discuss routing later in the tutorial.
If we now consider the other principle components we can go ahead and place U1 (dsPIC33),
U2 (I2C memory), U3 (temp/humidity sensor) and U4 (dual op-amp) in exactly the same way,
such that we end up with something like the following screenshot.
dsPIC33 board so far...
Note that the S08 footprints used for the U2, U3 and U4 components have been rotated
appropriately to reduce ratsnest length. This is best done at placement time as the ratsnest
display will update live to give visual guidance.
Start by placing U1 in the normal way and then start placement of U2 by left clicking once on
the Editing Window. Now use the ‘+’ and ‘-‘ keys on your numeric keypad to rotate the
component as you move it into position, left clicking the mouse again to commit placement as
before. Repeat the process for U3 and U4, moving or rotating parts after placement (right click
and then context menu options) until your board approximates the previous screenshot.

PCB Layout
111
If you are placing components in a high density area where routing space is at a
premium you can hide the part reference via the edit component dialogue form
(right click on the part and select edit properties from the resulting dialogue form).
Generally speaking you have two options for placement of the board. You can either manually
place the components in their positions or, if you have the Advanced Features Set (Proteus
PCB Design Level 2, Level 2+ or Level 3), you can use the Auto-placement feature to get all the
components on the board and then move them into the desired locations. In either case, you
may find it useful to temporarily disable the ratsnest lines during placement; remember that this
is controlled from the Layers dialogue form as discussed earlier.
The auto-placer can be invoked from the Tools Menu in the PCB layout and for our purposes all
the default options will suffice.
Selecting the Auto-Placer from the Tools menu
Whichever route you follow the task is to lay out all the components on the layout, using the
previous layout as a reference. Try to leave some space at the bottom of the board so that we
can run traces down and along from connector J2.
The following points are useful to bear in mind as you continue placement:

112
The middle mouse will zoom you in and out as you place components (as will keyboard
shortcuts F6 and F7)
Right clicking on a component once placed will present a context menu option, allowing
you to move, rotate or delete the part.
Changing the snap settings to a finer grid will allow more accurate positioning at the
expense of more precision being required to select the part.
If you place a part in an illegal position (e.g. over another part) you will get one or more
design rule violations. For now, simply move the part to a legal position – we will look
more closely at design rules in the next chapter.
DRC errors
Once you feel comfortable with placing and moving parts, feel free to move on to
the next section. We will load a board with all the parts placed before we discuss
design rules and routing.
Mounting Holes and Pad Styles
Before we move on to look at connectivity considerations we should complete the physical
layout by placing mounting holes for the board. In our case we want to use pad with 3mm hole
and a diameter of around 0.18in and to position them conveniently for mini-locking PCB
supports. The first thing we need to do is switch into circular through hole pad mode and scan
for a suitable pre-supplied pad in the Object Selector.
Select the correct pad style for mounting holes

PCB Layout
113
The nomenclature of pads in the PCB Layout is designed for easy reading and tends to follow
the following format:
<PAD TYPE> - <DIAMETER/SIZE> - <HOLE>
Units are in imperial unless prefixed with an ‘M’ so for example a C-40-15 is a circular pad with
a 40th diameter and a 15th hole and a C-200-M3 is a circular pad with a 0.2in diameter and a
3mm hole. Our spec requires a pad with a 0.18in diameter and a 3mm hole, which we can see
does not exist in the pre-supplied set. We therefore need to create the pad as follows:
1) From the Library Menu select the New Pad Style command.
2) Enter a name for the pad; we recommend you follow the standard naming convention (i.e. C-
180-M3).
3) Specify the pad type – in our case we want Circular through hole pad.

114
4) The diameter of the pad is 180th or 0.18in.The drill mark is the size of the mark output in a
drill plot, 30th would be fine. The drill hole needs to be 3mm and the guard gap should be
enlarged to 20
th
. The guard gap (or solder mask expansion) is the amount by which the pad
diameter is expanded on the resist plot.
5) At the bottom of the dialogue form we have the choice whether to make this pad style
permanent for future designs (Update Defaults option) or local only to this design (Local Edit
option). Unless there is a particular reason for a local edit only we recommend that you leave
this on the default setting.
6) When you exit the dialogue form you should see that the new pad style is available for
placement from the Object Selector.
When entering specific values you may find it easier to simply type in the values that you want
rather than using the up and down arrows beside the controls.
We are going to want to place two mounting holes at the top and bottom left of the board and
then a third at a specific location (for mini-locking PCB supports). You may therefore have to
move some circuitry out of the way to make room; for example, the crystal block at the bottom
or the pressure transducer at the top. As we’ve seen earlier we can easily do this by entering
selection mode, drawing a selection box around the circuitry and then dragging to a new
position. This is shown below with the crystal circuitry.

PCB Layout
115
Moving a selection of circuitry
Remember that you can resize the selection box to include or exclude items using the drag
handles if you don’t get the right size the first time.
Once you’ve cleared some space, go to the circular PTH pad icon again, select theC-180-M3
Pad style and place two at the top and the bottom left of the board.
Mounting holes placed
We want to position the third mounting hole above the battery and in a reasonably accurate
position. Specifically, we want to place the hole 35mm up from the bottom of the board and
87.5mm along from the left. We’ve already set our global origin to the bottom left of the board so
this is set to be the reference point for the co-ordinate system. All we need do therefore is move

116
the mouse up and right from the bottom of the board edge until the co-ordinate display reads
correctly (you may need to switch into Metric units using the ‘M’ shortcut key toggle).
If required, we can move the DC/DC converter circuitry as before, then switch back to pad mode
and place the final mounting hole at the correct co-ordinates.
Alternatively, having set the output origin and knowing the co-ordinates you can
right click on the mounting hole and select the move-to command from the context
menu to programmatically position the part.
With position sensitive components it is often useful to ensure that they cannot be nudged or
moved inadvertently after placement. You can lock any object in position by moving the mouse
over the object until it is encircled by a dashed line, right clicking on the object and selecting
Edit Properties from the resulting context menu. The Lock Position checkbox can then be
selected to prevent movement or deletion of the part.
You can also set a specific minimum zone clearance for the pad to reserve some
extra space for the bolt.
Locking pads and components
We have now completed the physical layout of the board. If you decided not to follow the full
layout process you can load a version of the board in its current form by opening the home
page, clicking on the Open Sample button. The project you want this time is the unrouted
dsPIC33 Recorder project from the Tutorials category.

PCB Layout
117
Opening a sample project
Design Rules and Net Classes
Now that we have a placed board we need to configure the software to obey any design
constraints or electrical considerations relevant to the layout. We can do this largely from a
single dialogue form called the Design Rule Manager. Start by launching this dialogue form now
from the Technology Menu in the Layout module.

118
Design Rules
The first tab of this dialogue form allows us to configure constraints and minimum clearances for
the layout. We have a DEFAULT rule loaded which must apply to all layers and all net classes,
providing a set of clearances between objects equivalent to manufacturing guidelines.
The Design Rule Manager
This rule and these clearances are created automatically for each layout in order to
provide a minimum set of constraints for a board. You can change the values of the
default clearances applied to new layouts via the Design Rule Manager on the
Technology menu.
The first thing we need to decide is whether a single rule is suitable for all layers and all traces
on the layout. It is possible to create as many new rules as required and we can limit their effect
to a given layer on the PCB, a specific area of the PCB and/or a given set of connections (net
class). A great deal of information on this is available in the reference manual but for our
purposes we can manage fine with configuration of the existing rule.
Given that this equipment is intended to work out-doors we’ll need to increase the clearances
between pads and traces to improve the insulation against condensing moisture. A 20%
increase should be sufficient so we need to change the Pad-Pad, Pad-Trace and Trace-Trace
clearances from 10th to 12th.

PCB Layout
119
Default clearance settings in the DRC manager
The graphics and edge clearances are fine at the default values.
Note that the edge/slot clearance field defines the clearance for power planes
against the board edge.
In addition to these clearances there is a board global rule for Resist-Trace clearance. This rule
enforces a clearance between the solder mask and copper and is intended to prevent exposed
slivers of copper on the manufactured PCB.
If, during route placement, you find these DRC errors, the solution is to either move the trace or
edit the pad style and change the guard gap (solder mask expansion) for that pad style.
Since there are no new rules required for this board we can move on to the net classes tab of
the dialogue.

120
Net Classes
This is the place where we configure trace and via styles and control which layers we route on
when auto-routing the board. The selector at the top allows us to switch between different net
classes and configure each separately.
Let’s start with the POWER Net class, which should be the default selection. As we discussed in
the Proteus Getting Started Guide any nets that include a power or ground terminal are
automatically assigned to the POWER net class, unless manually overridden.
We’ll set the track / trace size to 25th, not so much for current considerations but to reduce track
impedance (we’ll also place a single low impedance ground plane later to help with this). In PCB
nomenclature this corresponds to track style T25.
The neck style – if configured – specifies the track style for necking (thinning) to help the track
pass through obstacles. Together with our design rule aware routing (which knows which
objects are obstacles) this is very powerful. When set, you can hold the SHIFT key during route
placement to toggle between necked and normal track styles which is invaluable in tricky or
dense routing.
Advanced necking: The SHIFT key is held down while routing the escape from the BGA and
then released to resume routing at normal track width.

PCB Layout
121
Our board is not likely to be complex enough that this will be an issue but we'll set the neck style
to 15th so that we can practice.
Given that we don’t really have current constraints the choice of vias is a tradeoff between the
higher manufacturing costs of smaller vias and the decreased routing quality of large vias. For
the current this circuit is dealing with and for a standard 1.6mm FR-4 support plated with 35um
copper, vias with the standard 0.4mm hole are a good compromise. For the power tracks we
need a suitable annular size and 40
th
is a reasonable choice. We can therefore set the via style
to be V40.
If you are not sure of the characteristics of a particular style, you can view them by
selecting the appropriate mode icon (via, track, pad, etc.), highlighting the style in
question in the Object Selector, and then clicking on the ‘E’ button at the top of the
Object Selector.
The options at the bottom of the dialogue form allow us to change the via type (clearly not
relevant on a two layer board) and also to change the colour or visibility of the ratsnest lines.
The latter can be useful if we are manually routing and wish to quickly distinguish between
power and signal connections.
The layer assignment pairs on the right hand side tell the autorouter which layers to route on for
multi-layer boards. Again, for our two layer board, there is nothing to configure here.
We should now have finished setting up the POWER net class – your dialogue form should now
be configured as per the following screenshot.
Specifying the Power net settings

122
Let’s move on to the next net class in the selector; the ANSW class. You may remember that we
specifically named this net class in the Proteus Getting Started Guide in order that the 5V
switched power supply for the analog circuitry (the output of the DC/DC converter) could be
handled separately in the layout. What we want for these connections is a track size larger than
the standard SIGNAL net class but smaller than the POWER net class, so let’s change the
Trace Style to T15 (15th track). For consistency, the neck style can also be T15 and we can use
a smaller via (with the same 0.4mm hole) by selecting the V30 Via Style.
Specifying the ANSW net settings
If you don’t have a V30 via style you can create one easily by going to the Library
Menu, selecting New Via Style and filling out appropriately.
Creating your own net classes is extremely simple and provides you with the
flexibility you need both with regard to trace and via configuration but also with
design rule constraints
The final net class we have is the standard SIGNAL net class that encompasses all non-power
and unspecified connections. We’ve deviated from the widely used “8/10 Rules” (8th trace, 10th
clearance) in order to compensate for outdoor usage but the standard 8th track width (style T8)
is fine. We can also set the neck style to 8
th
and keep our standard V30 via style for these
connections.
Having finished configuration, exit the dialogue form to return to the layout.

PCB Layout
123
Keepout Areas
We can also introduce tracking constraints by limiting areas in which tracks can be placed. A
good example of this is the crystal towards the bottom left of the layout where we do not want
tracks under this area. To form a keepout area, start by selecting the 2D Box graphic icon and
changing the layer selector to be keepout.
Selecting the Keepout layer
Next, place a small box around the silkscreen of the crystal in exactly the same way as we did
for the board edge (left click to start placement, drag out the area, left click again to commit
placement).
Keepout placed produces 2 DRC errors
Unless you are very skillful you will be presented with a box indicating that design rules have
been detected.

124
First DRC warning
Checking the box on the dialogue form will prevent it from appearing in the future. If you left
click the mouse on the DRC section of the status bar a small window will appear providing
information on the errors. You should see that they are of type PAD-EDGE as the pads of the
crystal are closer to the keepout graphic than the 15
th
specified in the Design Rules.
Displaying DRC errors
We have two options here:
1) Ignore the DRC errors. The keepout graphic will not impact on connectivity.
2) Move the graphic to a legal distance from the pads. The easiest way to do this is to first
change the snap level down (View Menu), right click on the graphic and select the Drag Object
context menu option, and then change the snap level back when you are finished.
When you are finished your keepout area should look something like the following screenshot.

PCB Layout
125
Correctly placed Keepout
The default for the keepout is that it applies to all layers. However, after placing the
graphic on the keepout layer, you can right click change it to apply only to a specific
copper layer from the resulting context menu. This can be very useful on more
complex or densely packed board.
We have a similar problem around the temperature/humidity sensor (U3). We are going to want
a slot machined on the board to cut the thermal path and reduce the measurement errors of the
sensor (we want to measure environment temperature, not the one conducted by the PCB). We
therefore need to ensure that no tracks are placed in the area we are going to slot through:
1) Select the 2D Graphics rectangle icon and then change the layer to be KEEPOUT.

126
2) Place a rectangle around the bottom half of the IC as shown below.
U3 with a Keepout
This time we cannot move the keepout to remove the DRC errors as the positioning is sensitive.
Instead we can manually override the errors by launching the DRC dialogue, right clicking and
selecting the Ignore option from the resulting context menu.
Ignoring DRC errors
Design Rooms
Alternatively, we can designate this area of the board to have different design rules from
everywhere else. To do this, we select the room icon and drag a box around the area. Then we
set it up as a DRC room which needs to cover all layers (since the keepout is on all layers) and
give it a sensible name.

PCB Layout
127
Setting up a Design Rule Room
Now that we have the room set up we need to change the design rules inside it. Go back to the
design rule manager and find the room definition. You'll notice when you select the room in the
tree that the right hand side shows you that the default rule but shaded in a light grey. This
indicates that the default rule applies in the area but was defined at a higher level. In other
words, the room inherits the clearances from the board unless you give it specific clearances.
We do this by clicking on the new button to create a new rule, give the rule a name and scope it
to apply to the room and finally setting the clearances we want. In our case we simply want to
turn off the edge clearance test in this area - everything else can stay the same.
Setting a new Rule for the Design Room.
Design Rooms are a really useful concept and helpful wherever clearances vary in
specific regions of the PCB. This can be as simple as pad-pad clearance on fine
pitch SMD devices, fanout areas from BGA's, edge connectors at the board edge
and so on. We strongly recommend you read up further in the reference manual.

128
Routing the Board
Having configured the board constraints we can now move on to actually making connections
and routing the board.
Teardrops
Teardrop functionality is included in the Advanced Feature Set and requires a
license for PCB Design Level 2 or higher.
Placing teardrops at the connection point between track and pad is often useful in preventing
drill breakout during board manufacture. We can configure teardrops from the Set Teardropping
command on the Technology Menu.
The dialogue form lets us set the maximum annular ring size on a pad below which a teardrop
connection will be made and then also lets us set the length of the teardrop. You can, if you
want, also apply teardrops to surface mount pads although we are not aware of any
manufacturing reason for doing so. On surface mount pads the annular ring parameter is
considered to be center pad to nearest pad edge.
A per pad override for setting/clearing a teardrop connection can be accessed from the edit
single pin dialogue. This provides an additional level of control over where teardrop connections
are made.

PCB Layout
129
Note that the creation of a teardrop connection is dependent on the design rules. If making a
teardrop connection would violate one of the design rules then it will simply not be created.
Once configured teardrops connections will be made dynamically as we complete routes in the
sections below.
Placing a Route Manually
Before we start, we will want the ratsnest lines turned back on. If you have them disabled (can't
see any green lines between pads), turn them on from the View Menu - Displayed Layers
dialogue.
Let’s begin by manually placing some tracks on the board. Typically, we would manually lay out
connections where a specific path is desired for the track or where we need greater control over
track position. On our layout we want to make sure that our connections from connector J2
follow a sensible path around the board so we can start here and route them manually.
Start by selecting track mode at the left hand side of the Object Selector and changing the layer
selector to be on Top Copper.
Trace / Track selection and the Layer selector
If we look at pad 4 of the J2 connector we can see that the closest ratsnest line is directing us
across to the GND pad on the step converter. This is not ideal as we would have to navigate the

130
mounting hole and then track into the small SMT pad. Instead, we will route this down and
across the bottom of the board to a more convenient ground connection.
The Layout module features a sophisticated 'follow me' routing algorithm for manual routing in
which the route being placed will follow the path of the mouse as best it can while still obeying
all of the design rules for the board that we set up previously. You start track placement by left
clicking the mouse on pad 4 and then move the mouse downwards.
Routing J2 Pin 4
You should see that the closest legal destination for the track is now highlighted in white. This
will update as we move the mouse and since we are not going to route to this destination we
can ignore it for now.
You will also see a shadow track between the current mouse position and the destination. If
you press the ENTER key on the keyboard it will complete the route along the path shown by
the shadow track. You can do this at any time while routing manually.
When the mouse approaches the bottom of the board, you could just change direction to the left
and the track will corner to follow the mouse. However, since we want a tighter corner it is better
to left click the mouse to place an anchor and then change direction to the left.
You will see that as we move further to the left the ratsnest guide will change to show us that we
can terminate the track on pin 1 of jumper JP2.

PCB Layout
131
Connecting to JP2 Pin 1
Once we are underneath the jumper we can change direction and move upwards towards the
destination pin
Connecting the trace to the pin
Finally, we can click left over the pin to finish placing the route. This will both commit the route
and remove the ratsnest line corresponding to this connection.

132
Finished route from J2 pin 4 to JP2 pin 1
Note that we did not need to select the width of track to route with as we configured this in the
previous chapter. The PCB Layout recognizes that we are routing a track on the GND net,
applied the rules for the POWER net class and selected the specified 25
th
track style for us.
Manual routing is probably the most common action you will perform with the software and it is
vital that you understand how it works. The basic rules of operation are:
Left click on pad, track or zone border to begin routing from that object.
Left click at any point during routing to commit the route up to the mouse position (we
call this anchoring).
Right click to terminate the route at its last committed / anchored point.
ESCAPE key to abandon route entry completely.
ENTER key will automatically complete the track in the path shown by the 'shadow'
track.
SPACEBAR to float a via on the end of the route and left click to then place the floating
via.
Double left click to drop a via at the current mouse position.
Move the mouse backwards over existing tracking to rub-out.
SHIFT key toggles the neck style on/off (SHIFT key down = neck style on, SHIFT key
up = neck style off).

PCB Layout
133
We strongly recommend experimenting with manual routing for a while on this board until you
are comfortable with how it works. The following is a summary of how to perform common
actions; try these while routing any of the remaining connections.
Panning and Zooming
While placing a track you can use the middle mouse wheel (or F6 & F7 keys) to zoom in and out
during routing. Panning will happen seamlessly when the mouse is at the edge of the Editing
window during routing.
Placing Anchors
The follow me routing algorithm will move the track being placed according to the way you move
the mouse. If you want a track to follow a particular path then you need to help by left clicking
whenever you change direction. This places an anchor or commits the route up to the mouse
pointer such that the follow me router will not change it. You will see this happening as the
outline track becomes solid.
Getting Stuck / Re-routing while routing
Since the manual routing system obeys the design rules for the board you don't need to worry
about clearances while placing routes. You can however route to a place where you are blocked
(the routing icon will change to a no-go sign at this point). Often you just place a via and
continue on but sometimes it is better to rewind and try another path across the current layer.
Moving the mouse backwards over the route being placed will rub out that portion of track so to
rewind and change direction just move the mouse back to the last good point - anything you had
placed from that point onwards will be removed.
On densely packed boards in particular, speed of mouse movement is an issue.
Remember that you are guiding the placement so moving slowly through tight
spaces will work far better than ripping the mouse from source to destination. Use
the SHIFT key to neck down and back up - this will get you through tight spaces.
Placing Vias
If you double click during placement you will place a via at the point the mouse is at and can
then continue routing on the associated layer. If you press the spacebar you will float a via on
the end of the mouse and can then position the via manually before placing with a left click.
Using the spacebar has the advantage of snapping to legal objects (e.g. via under SMT).
In either case the placement of the via is also design rule aware and Proteus will not let you
drop a via in an illegal spot. If you use the floating via method (with the spacebar) the layout will
attempt move the via to the nearest legal spot. This can be extremely useful on busy boards or
when you want to butt a via tightly against another object.

134
Layers used for vias are defined in the Layers Pairs dialogue on the Technology Menu.
Examples of routing with vias and discussion on layer pairs follows further in the tutorial.
Object Hugging
Since the design rules are all live during placement it is quite easy to hug a track to another
track or to wrap a track around an object. If the mouse is over an object where the route being
placed cannot travel then the route will follow the mouse path as closely as it legally can,
essentially hugging the barrier object.
Abandoning a Route
- If you want to abandon the route at the last committed (solid) segment then right click the
mouse.
- If you want to abandon the route at the mouse pointer then left click to commit up to mouse
pointer and then right click to terminate the track.
- If you want to abandon the route completely then hit the ESCAPE key.
Making Connections
If you are connecting directly to a pad then a left click of the mouse will complete the connection
and terminate route placement.
If you are connecting to a track then left click will commit the placement and right click will
terminate the route forming the connection. The same procedure applies if you are connecting
to a zone except that you must connect to the zone border.
Placing a Curved Route
Placing a route with curved corners can be helpful with signal integrity and net tuning or simply
for aesthetic reasons. In Proteus, you can switch to curved route placement by holding down
the CTRL key during route placement. Releasing the CTRL key will immediately switch back to
linear routing giving you the control to curve only specific parts of the route. The process of
placing the route is exactly the same as before, except we hold CTRL down on the keyboard for
curves. So:
1) Left Click the mouse to start the route.
2) Hold CTRL down to curve the corners and guide the route towards the destination pad
with the mouse.
3) Left click the mouse on the destination pad to terminate the route.

PCB Layout
135
Deleting a Route
Once the route has been completed we can delete either the full route or a specific part of the
route if we are not happy with the placement. Let’s assume that we were not happy with our
placement of the last piece of track (upwards to pad 1 of JP2).
Start by right clicking on the track over this segment of track. This will highlight the entire track
and the Delete Route option near the top would then remove the complete trace from the board.
However, we have far more control if we use the options at the bottom of the context menu. In
this particular case, select the Trim to Single Segment option; this will change the selected area
of track to the segment we have clicked on.
Trimming a trace to a single segment

136
Next, right click on the highlighted segment and select the Delete Route command; this will
delete only this segment of the route.
Deleting a trace via the context menu
Finally, zoom in, change the snap settings if need be and replace the route from the existing
track to the terminating pad.
If things have gone more badly wrong you can simply delete the entire route and start again;
what you are aiming for is something like the following screenshot:

PCB Layout
137
Editing a Route
It is often the case that routes need to be nudged or moved into position after placement and we
definitely don’t want to be deleting and replacing routes or parts of routes all the time. To take
an example, let’s move our track lower down the board a little, towards the bottom board edge.
Start by right clicking on the horizontal section (segment) of the track; this is the section we
want to move. Next, select Drag Route from the resulting context menu, move the mouse down
to ‘pull’ the track into the desired location and then left click again to commit placement.
Moving tracks works as we’ve seen on a track segment. Using the Trim Manually
option on the context menu for a track allows you to define your own segment and
you therefore have complete flexibility with altering track topology.
You may want to perform operations on multiple tracks at one time. The obvious example of this
is changing the width of the track(s) and/or the via style used when routing them. You can do
this by first switching to selection mode, then using CTRL+left click to select and finally by right
clicking on any of the selected tracks to access the context menu.
Layer Pairs and Manual Routing
The track we have placed is of course only on top copper, whereas we often want to via up and
down through the board when routing. Proteus handles this with a concept called Layer Pairs.
This means that every layer on the board has an associated layer so that via destinations are
known during placement. For a two layer board this is obvious with top copper being associated
with bottom copper and vice versa but with multi-layer boards configuring the layer pairs
(Technology Menu – Layer Pairs) can be an important step.
Don't be surprised to see much of layer pairs dialogue disabled. The available layer
pairs are restricted to the signal copper layers set up in your layer stack.
In our case, the default assignments are correct and no action is required. Let’s place a couple
more routes manually to see how this works. We’ll look at connecting pins 1 and 2 of the J2
connector which are the transmission lines from the USART on the dsPIC processor.
We’ll start with pin 1 and route from the pin on the bottom copper layer. Make sure that you
have track mode selected and then hit the space bar on the keyboard, noticing that this will
toggle the layer between the two layers associated as a layer pair. If you have ended up on top
copper simply hit the space bar again to set the layer to bottom copper.

138
Selecting the Bottom Copper layer
The processor is some distance from the connector and the easiest path would seem to be
down and along the bottom of the board. Begin placing the track by left clicking on pin 1 on the
connector and then moving the mouse downwards
Routing on Bottom Copper
When we get near the bottom of the board, left click the mouse to place anchors and guide the
mouse to the left. To maximise space on the board you can route across the bottom of the
board with the mouse over the board edge graphic - this will hug the track to the absolute edge
of the board leaving only the Edge Clearance between the two.
Tracks will hug the board edge
Once you get near the U1 IC bring the track up just past the right hand pads of the processor
footprint.

PCB Layout
139
Routing to the left of the right hand pads of the Processor
We now need to place a via before we can connect to the SMT pad on top copper. As described
above you can either double click the mouse at the point you wish to place the via or you can
press the spacebar to float a via and then guide the placement point with the mouse before left
clicking to commit. The latter method has the advantage of allowing you to butt the via as
closely as possible against the pad thereby minimising the stub track length on top copper.
Placing a via by pressing the space bar
Quite a lot has been covered in making these connections and, unless you are fairly skillful,
there has probably been some finger trouble along the way. We’ll continue with the other
connections from the J2 connector to help familiarize ourselves with the techniques we’ve
introduced.
Pin 2 of the connector should follow an almost identical path to pin 1 and again we can start
placement on bottom copper (check the layer selector before you start placement; the space
bar will toggle the layers). We can easily hug the track we have just placed by moving the
mouse parallel to the path we want to travel but over the original track as shown below.
Tracks will also hug other tracks

140
In order to make the connection, we can then route vertically underneath the pads and make a
short 45 degree track before double clicking to place the via and complete the connection.
Routing a 45 degree angle
Of course there are many ways we can route the board and personal preference also plays a
part. Feel free to experiment with the other connection on the connector, working around the
battery holder, using the ratsnest to find a legal destination and then completing the route. The
following screenshot is an example of what you might have when you are finished.
Both tracks fully routed
Basic Auto-Routing
From this point on we’ll use the auto-routing engine to complete placement of the routes. As
with the manual tracking the auto-router will obey all the design rules that we configured earlier.
Start by invoking the auto-router from the Tools Menu in Proteus (PCB Layout Module) or from
the icon at the top of the application.

PCB Layout
141
Select the Autorouter from the Tools menu
The resulting dialogue form is reasonably complex but all fields have context sensitive help
associated with them. You can also find additional information about the various type of routing
pass in the reference manual. For our purposes (and indeed for most boards of small/medium
complexity) the defaults are more than adequate. We’ll start by running in ‘fully automated
mode’ which should be selected by default so simply hit the begin routing button to complete the
remaining connections.
The Autorouter dialogue form

142
Everything will happen quite quickly from this point onwards but you should see routing
progress on the status bar as the engine works towards completion. Once the board is complete
there are two immediate points of note:
The auto-router has preserved those tracks that we placed manually and has not ripped
and replaced them whilst working on the rest of the board.
Once the autorouter has completed a final pass is made to corner the tracks. If you prefer
this not to happen you can remove the Recorner Pass option on the dialogue form before
invoking the router
Set the Recorner Pass to be NO
Length Matching Routes
Automatic length matching is part of the advanced feature set and requires PCB
Design Level 2 or higher.
For high speed signal lines it is common to need to match the lengths of the tracks to ensure
that all relevant signals arrive inside the sample and hold time of the receiving chip. While not
required for the tutorial design we now have a fully routed board so it is a good opportunity to
explain how the feature would be used. The first step is to select the tracks that you wish to
length match by holding the CTRL button down and left clicking on each track. We've chosen to
do this with two large routes into U1 as shown here:

PCB Layout
143
Selecting two tracks for length matching
Next, right click on one of the tracks and select the match route lengths command from the
context menu. If successful you will see track segments added in a serpentine pattern to the
shorter route in order to match its length with the longer route.
Matched lengths
Full configuration of the added length can be found on the Configure Length Tuning command
on the Technology Menu or from the context menu.

144
Configuring Length Matching Options.
Other points to note about length matching.
You can match multiple tracks at the same time (e.g a bus).
The length of a track is shown on the status bar when it is selected.
If a track is part of a group that has been length matched the target length is also shown
in the status bar when you select the track.
The pre-production check will test all matched tracks against their target length and warn
you if their length has changed.
If you choose routes with vias the length (depth) of the via is calculated from the
thickness values you enter in the layer stackup.
The Selection Filter
Now that we have a completed board it’s worth spending a little time looking at the techniques
for selecting various object types on different layers.
The Proteus Layout module uses the Selection filter at the bottom left of the application window
to determine which objects are available for selection at any given time.
The left most button will determine whether the layer selector is active:
When this is toggled off the selection applies to all layers on the board.

PCB Layout
145
When toggled on the selection applies only to the layer specified in the layer selector
The other buttons represent different object types (tracks, components, graphics, etc.) and
determine whether those object types are selectable. Hover the mouse over an icon for a tooltip
description.
If you switch between the different modes of operation (for example from selection mode to
track mode to component mode) you will see that the selectable object types will change
according to the mode you are in. Whilst these are good defaults for normal operation you can
change at any time simply by toggling on or off the layer switch or object type that you do or do
not want to be selectable. If you find yourself changing selectable items regularly you can also
change the defaults via the System Menu – Set Selection Filter command.
The Layer Selection options
Let’s take a practical example and delete all the traces on the top of the board, except the one
we have manually placed. Start by entering Selection Mode and left dragging a selection board
around the entire board.

146
Select the entire board
Next, deselect those objects that we do not want to delete, namely everything apart from tracks
and vias. The tagged items will update automatically to provide visual confirmation of what is
selected.
Only the tracks will be selected
Now change the layer to be Top Copper on the layer selector and toggle the layer button such
that the selection filter applies only to the current layer
Top copper selected
Use the green drag handle at the right of the tagbox to move the selection filter in until it does
not encompass the J2 connector.

PCB Layout
147
Notice that Only the traces on Top Copper are Selected
Finally, use the icon at the far right of the selection filter to deselect items that are only partially
inside the tagbox; in our case this will deselect the track we manually placed from J2, pin 4.
Tag box toggle
We can now simply hit the delete button on the keyboard or right click inside the tagbox and
select Block Delete icon to remove all the top copper tracks.
Bear in mind that the selection filter controls what objects are available for selection
at any given time. If you ever find that you can’t select an item the first thing to
check is whether that object type is enabled for the mode that you are in.
Alternatively, simply switch to Selection Mode where all items are selectable.
Advanced Auto-Routing
Given that we’ve ripped a lot of partials and removed vias as well we’ve actually made a bit of a
mess here. Fortunately, we can fix the situation by simply re-invoking the auto-router and re-
placing all our tracks. The router has its own clean up phase so it will tidy up all the redundant
partial tracks for us as it completes the new routing.
If you have a standard features version of Proteus (PCB Starter Kit, Level 1 or Level 1+) simply
run the autorouter as we discussed in the previous section to re-route the board.
For those using the Advanced Feature Set, we’ll use this section to show in brief some of the
additional features available. These fall into two main categories:
The ability to route only a specified area or set of connections.
The ability to control the routing script; i.e. to determine which routing commands are
executed and in which order.

148
Start by invoking the autorouter dialogue form (Tools Menu), switching to Interactive mode and
then selecting the Begin Routing button.
Entering the router interactively
A command window will open at the bottom of the Editing Window, which will allow us to direct
the routing progress interactively. The PCB Layout provides a rich command set to control
routing, including such things as bend radius for mitering tracks and fanout length and direction
from SMT pads. This is fully documented in the reference manual so we will concentrate on
some basic practical examples in this tutorial.
There are a couple of important points worth emphasizing at this stage:
Any commands entered will action on a set of tagged connections or on the whole board if
nothing is highlighted.
Changing the circuit or switching modes will automatically exit the routing interface.
Essentially, what this means is that we can dictate what connections are routed by controlling
which items are highlighted.
First of all let’s clean up the loose tracking on bottom copper resulting from our previous rip of
the top copper tracks. The basic syntax of most commands is:
<command> <number of passes>
so we can start by typing clean 2 to clean up the superfluous tracking.

PCB Layout
149
Next, let’s assume that we want to route all the VCC connections. Select the
VCC/VDD=POWER net in the Object Selector and click on the small ‘T’ button above the Object
Selector to highlight all the connections on that net. Finally type in ‘route 5’ to route these
connections.
Clicking anywhere in the Editing Window will deselect the currently tagged items.
When the focus is in the Editing Window you can also use the middle mouse (or
keyboard shortcuts) to zoom in and out in the normal way.
Similarly, we can highlight connections on an area of the board and route them independent of
the rest of the board. For example, right depress the mouse and drag a selection box around
the left half of the board and then type ‘route 10’ to complete open connections in that area.
Autorouting an area of the board
You may notice that this has left a couple of ratsnest lines or has not completed all of the
connections. We could try to resolve this by issuing clean, filter and more route commands, but
for our purposes it’s easier to simply revert back to a ‘whole-board’ scenario and then

150
completing routing. You can do this by left clicking on an empty area of the Editing Window to
clear the selection. Typing route 25, followed by clean 2 should see the board completed
Finally, we can reduce trace length by typing recorner diagonal as a finishing touch.
Do note that there is much more flexibility in the command set than that shown in this tutorial,
both in the number of commands and in the parameters that control the command actions.
You can exit auto-routing at any time via the ESCAPE button on your keyboard.
Netlists and Design Changes
We have now placed and routed our layout based on the schematic we designed in the Proteus
tutorial. In practice however, it is very unlikely that we would not be making design changes
during the PCB process so we'll devote a little time to examining a typical workflow.
Clearly, we will be editing both the schematic and the layout modules so both need to be open.
If the schematic tab is closed you can open it from the application module toolbar at the top of
the Proteus application.
Proteus icon on the Application toolbar
Since we will be working with both modules you may want to split them into two frames if you
have two monitors. To do this simply drag one of the tabs onto the other monitor. For this
documentation, we will assume that the Schematic Capture and PCB Layout are open as tabs
inside a single Proteus frame.
Multiple tabs in one frame

PCB Layout
151
Live Netlisting
First, let’s delete the J2 connector on the schematic. Switch to the Proteus tab, right click and
select delete object from the resulting context menu.
Deleting a component in Proteus
Now switch back to the PCB tab. Note that the J2 part has been dimmed to show that it is not
present on the schematic and that the connectivity status shows that we have pending changes
(we are out of sync).
Netlist is out of sync
Since the action taken in Proteus removes from the board it requires manual confirmation. We
can now either hit undo (CTRL+Z) if we don't like the change or we can click on 'Changes
Pending' in the connectivity status to accept the change. When we do this, the 'shadow' part will
disappear.
Clicking on Changes Pending will remove J2 and correct the netlist
Note that tracks that were connected will also be deleted. If you want instead to
delete only the footprint (leaving the connected tracks in place as stubs) then you
can do so by directly deleting the package in the layout.
The undo system is still available to revert the changes. Clicking on the UNDO icon (or
CTRL+Z) once will bring back the shadow objects and repeating the process a second time will
bring back the schematic part and the real PCB footprint.

152
Undo and Redo icons
If you click on undo while in the PCB Layout tab but the undo action applies to the schematic
you will be prompted to confirm the operation. In our case, we do want to bring back the
connector so accept the prompt to return the PCB to the original state.
This is a simple example of a change which affects objects already placed on the layout. The
important thing to remember is that while the netlist is live, you must manually confirm any
change which affects the connectivity of objects you have already placed.
Batch Netlisting
If you prefer, live netlisting can be turned off and a more traditional batch mode netlist used.
This is controlled from the 'live netlist' toggle on the Tools menu (in the PCB module).

PCB Layout
153
Having turned live netlisting off, let's repeat the same procedure to see the difference. Switch to
the schematic tab, delete the connector and then switch back to the PCB tab. This time the
connector on the PCB remains present and the connectivity status reports that the layout is
locked and out of sync.
Status bar messages when 'out of sync'
This means that we have not loaded the changed netlist and cannot work on the layout until we
bring the netlist across. Proteus works with a single database of parts that include schematic
components and pcb footprints so - while you can work on the schematic - you cannot work on
the PCB until you sync it with the schematic. Click on the connectivity status to unlock the PCB
and bring the current netlist across.
This brings us to the same state as we arrived at automatically with live netlisting on. We have a
shadow part in the layout and the connectivity status reports changes pending.
The main difference between live netlisting and batch netlisting is only that you must confirm
each netlist load manually in the latter mode. We recommend that live netlisting is used for
normal working, although for particularly large designs batch mode may provide a useful tool.
Some functionality will require a live netlist and so if you are working in batch mode
you may find menu commands disabled until such time as you bring the netlist back
in and sync.
Annotation
Annotation changes from schematic to layout or from layout to schematic are also a common
editing operation when both modules are in use.
Schematic to PCB
Annotation changes made in the schematic will automatically be reflected in the PCB when live
netlisting is on and will require unlocking when live netlisting is off. The Global Annotator on the
Tools Menu on the schematic can automate this task.

154
PCB to Schematic
You can re-annotate the board either manually (editing the part reference labels) or globally
from the automatic annotator command on the PCB Layout tools menu.
Launching the Automatic Annotator
When live netlisting is on, this will automatically reflect to the schematic. With live netlisting off,
the schematic will update and the layout will then lock as the netlist has changed and needs to
be manually passed through to the layout.
General Netlisting Rules
There are several important rules of thumb to understand about netlisting in Proteus.
When live netlisting is on, a change that adds connectivity will happen automatically (e.g.
adding a wire on the schematic will add a ratsnest on the layout). If you make a change that
removes connectivity the layout will show the change by dimming the deleted objects and you
will need to manual confirm the operation.
When live netlisting is off (batch netlisting) any and all changes to the netlist will require you to
unlock and apply the netlist before you can continue working on the layout.
Clicking on changes pending to remove footprints that have been deleted on the schematic will
also remove associated tracks. If you want to remove footprint only and leave the tracks simply
delete the part in the layout (rather than Proteus).
Dimmed objects in the layout are visual placeholders only - they do not exist on the board. Best
practice is always to click on changes pending on the connectivity status and to arrange the
layout to conform to the schematic.
Imported projects (from older versions) will always start with live netlisting off as there is no way
to tell whether they are in sync. By contrast, new projects will always start with live netlisting on.
In either case you can switch according to preference from the live netlisting toggle on the Tools
menu in the PCB layout module.

PCB Layout
155
Power Planes and Slots
If you switch back to the layout tab we will continue the layout phase of the project. To minimize
track impedance we are going to place a power plane covering the entire board.
Placing Power Planes
This is actually the easiest type of power plane to place and is available in all levels of the
professional software. Start by invoking the power plane generator command from the Tools
Menu
Opening the Power Plane Generator from the Tools menu
From the resulting dialogue form select the GND=POWER net, keeping the layer as bottom
copper and setting the boundary style to be T10. This is the trace style in which the inner and
outer boundaries of the zone are drawn and also determines the thinnest section of copper by
which the power plane can make a connection. Setting this larger will prevent the copper
flowing through small gaps (e.g. between pins) but making it smaller means that connectivity
may be made only by thin sections of copper.
We can leave the clearance between the power plane and the board edge at the default value.

156
Power Plane Generator Dialogue form
After you exit the dialogue form you should see that the power plane is generated across the
entire board.
Power Plane has flooded the entire layer
The clearance from the zone to the board edge is defined by the Edge/Slot design rule. We can
change this via the Design Rule Manager on the Technology and the zone will re-generate to
the new clearance when we have finished.

PCB Layout
157
Since you can set a new design rule per layer it is possible to have different
clearance rules for power planes on different layers
Stitching Zones
In Proteus you can auto stitch / shield a power plane. This is done by right clicking on the edge
of a power plane and select the relevant option:
Nesting and Islands
There are several additional configuration options available to us now that we have placed the
zone. Editing a zone is slightly different from most other objects in the PCB Layout, in that you
must right click on the border of the zone (to avoid continuous unwanted selections).
Firstly, check the selection filter and make sure that the zone object type is selectable (or switch
to selection mode).

158
Zone icon in the Selection Filter
Next, zoom in and move the mouse over the edge of the zone, right clicking the mouse when
the zone is shown as active under the mouse. Select the Edit Properties from the resulting
context menu.
Right click on the edge of a zone to edit its options
The main options of interest are towards the bottom of the dialogue form and are explained
below:
Relieve Pins
When checked pins on the same net as the zone will have thermal relief applied to them; the
thickness of the thermal relief is determined by the Relief field of the dialogue form.
The software will prevent you from using a relief track style that is larger than the
boundary style thickness; this is to protect against the reliefs 'sticking out' of the
boundary.
The topology of the relief stems on a particular pad can be changed to a diagonal
'X' by editing the pad itself after placement. This is sometimes useful to maximise
contact with a zone.
This option should almost always be left in its default checked state.
Exclude Tracking
If this option is checked, the zone will treat tracks on its own net as obstacles. Otherwise the
zone flows over such tracking, effectively ignoring it. Tracks on other nets, or loose pieces of
track on no net are always treated as obstacles.
This option is normally left unchecked.

PCB Layout
159
Suppress Islands
An island is defined in the PCB Layout as a block of copper or zone area in which no valid
connections can be made. When checked, the layout will remove all such blocks from the
board, leaving only areas of copper with connections.
Allow Nesting
It is quite common, particularly with larger boards, that the flow of a zone will encounter an
obstacle through which it cannot pass. When checked, the zone will jump over the obstacle and
continue flowing across the board.
This is a very useful option for example on busy boards or where you want to connect a pad
where the topology of the board makes it impossible for a single zone flow to get through.
Given our relatively simple board, the default options are ideal for our purposes. Selecting the
nesting option will have no effect for example as there are no inner boundaries on the board.
However, if you want to experiment you should find that if you uncheck ‘suppress islands’
option, the resulting zone populates far more of the board that in our initial configuration.
We have covered only the basics of power plane functionality here relevant to our current
design. For more information, including split planes, zone keepouts, and bridge tracking please
see the power planes section of the reference manual.
Slots
To complete the layout of the board we need to return to our temperature/humidity sensor (U3).
In order to make accurate measurements, we want a thermal cutout around this part, ensuring
that the temperature we are measuring is actually the environmental temperature and not
conducted heat from the PCB.
You may remember that we placed a keepout area around this part to prevent the autorouter
from placing tracks through the area we want to cut out. Start by zooming in around U3 and

160
removing the keepout. You’ll need to either switch to Selection Mode or to change the selection
filter such that you can select 2D Graphics
Deleting a Keepout area
While we are here, we might as well move across and repeat the process by deleting with the
other keepout around the crystal.
Returning to U3, we now need to outline the cutout region. In the PCB this is a two stage
process; we need to place graphics appropriately on a mechanical layer and then designate the
mechanical layer as the slotting layer when we generate output for manufacture.
Select the 2D Graphics Line icon, change the layer selector to be MECH1 and then place three
lines to form a ‘U’ shaped cutout.
Placing a slot on MECH 1
Finally, we can thicken these three lines to something more appropriate as follows:
Enter selection mode, hold the CTRL button down on the keypad and left click once on each
line. This will select all three lines
Selected items are white

PCB Layout
161
Right click on any line and select Edit Properties from the resulting context menu.
Uncheck the Follow Global checkbox, change the width to be 20th and then apply to all tagged
graphics.
Changing multiple objects at once
We will cover how to specify MECH1 as the slotting later in the documentation in the
section on manufacturing outputs.
3D Visualisation
Now that the board is now routed and ready for production we first want to examine it in 3D in
order that we can properly preview how it will look in real life and possibly make final design
alterations prior to prototyping. Start by invoking the 3D Visualisation Engine from the module
toolbar at the top of the application
3D Viewer icon
This will open and load the 3D view of the board in a separate tab. As with any tab, you can
drag onto a separate frame if you want to look at both the 2D layout and the 3D view
simultaneously.

162
Basic Navigation
The first thing we can do is view the board from different preset angles. Five preset views are
supplied: top view, front view, back view, left view and right view and these are accessible via
any of the following methods:
Menu options on the View menu in the 3D Viewer
From the navigation toolbar at the bottom of the 3D Viewer
From keyboard shortcuts F8 through F12 whilst in the 3D Viewer.
Now that we can look at the board from a number of angles the next thing is to be able to look
at it at a specific zoom level. Again, there are numerous ways to zoom in and out of the board:
Roll the middle mouse wheel in and out (recommended)
Menu options on the View menu
From the icons on the Navigation Menu
From keyboard shortcuts F6 (zoom in) and F7 (zoom out)
Experiment now with custom zoom levels and different preset views – whilst it is pretty
subjective we envisage most users changing views via the navigation toolbar or keyboard
shortcuts and using the middle mouse wheel to zoom in and out.
Bareboard View and Height Clearances
For inspection of resist and hole depth it is often useful to view the board without components.
Selecting the bareboard view will remove all the physical components from the board.
Show Components icon
By contrast, if you need to fit the PCB into a chassis and wish to check height clearances you
can enable the height boundary box via the icon at the bottom of the display.
Casing icon
Specification of the height takes place from the Dimensions command on the Settings menu of
the viewer.

PCB Layout
163
Board properties dialogue form
Custom Views
The next logical step is to be able to customise the view. This works conceptually by ‘attaching’
the mouse to the camera such that as you move the mouse the camera moves to the area of
the board that you are interested in. You can invoke the Navigation mode either from the View
menu, the crosshairs icon on the Navigation toolbar or simply by clicking the left mouse button.
3D Mouse cursor
You will know as soon as you are in Navigation mode as a crosshair cursor will appear over the
mouse and your view of the board will change as you move the mouse. Using this together with
the middle mouse wheel zoom will allow you to both ‘fly pass’ the board and to easily zoom in to
closely examine a particular area of the board. Exiting navigation mode is as simple as right
clicking the mouse.
For example, if we start in Front View (use the F9 keyboard shortcut) and we want to examine
the resistors on the right we might proceed as follows:
1) Left click the mouse to enter navigation mode.
2) Move the mouse over the resistors.
3) Roll the middle mouse button to zoom in as required.
4) Right click the mouse to exit navigation mode.
The final necessary piece to completely customize the view is to allow users to spin or ‘orbit’ the
board. This is done in navigation mode by holding down the left mouse button and moving the
mouse. Essentially this will spin the board as you move the mouse – when you release the

164
mouse button the camera will follow the mouse around the current view of the board as normal.
Try this now, experimenting with different views of components on the board.
Remember that, if you are struggling to get the view you want you can use the keyboard
shortcuts or navigation toolbar to return to one of the preset views. You should find however,
that with only a little practice you become quite proficient at navigation.
To summarise:
Left click enters navigation mode.
Camera follows mouse around the board in navigation mode.
Using the middle mouse wheel (or shortcut keys) allows you to zoom as you move the
camera.
Left depressing the mouse in navigation mode allows you to spin/orbit the entire board.
Right click of the mouse exits navigation mode.
3D Models (STEP/IGES)
Each footprint on the layout can also have an associated 3D model. Normally, these are either
STEP Files (for large or complex parts) or scripted geometric models (for simple passives).
In the case of STEP or IGES files, the procedure is:
1) Download the file from the internet or otherwise source the 3D model. There are many sites
available, with www.3dcontentcentral.com and www.tracepartsonline.net being amongst the
most popular.
2) Save the file into the MCAD directory of your Proteus installation. By default, this is:
C:ProgramDataLabcenter ElectronicsProteus 8 ProfessionalMCAD
3) Right click on the footprint in the PCB and select Make Package, and then click on the 3D
Mechanical Models tab.

PCB Layout
165
4) Type the name of the STEP file and then the rotation and offset required to align the STEP
file with the pads on the board.
For geometric models, the difference is basically that you describe the part in terms of size and
shape via a simple scripting language. This is covered in the reference manual.
Live Update
Like any other module in Proteus, the 3D Viewer will update live as changes are made to the
PCB layout module. In practice, the usefulness of this will depend very much on the power of
your machine (number of cores, memory, etc.) and the complexity of the board.
On a board of modest complexity and a modern computer the redraw time is not significant and
- particularly on split frames - is very useful for movement and positioning.
More information on 3D Visualization including creation your own 3D models, exporting
3D STEP Files for MCAD import, customizations and applying 3D data to legacy designs
can be found in the 3D Viewer section in the online reference manual.

166
Board Output Options
Last, but by no means least, we come to the crucial business of reproducing the pretty on
screen graphics on paper or film. Under Windows, most hard copy devices are supported
through the normal Windows printer drivers. Additionally, we supply our own drivers for pen-
plotters, Gerber photoplotters and Excellon NC drill machines.
Printing
We will deal here firstly with printing to an ordinary Windows printer device – it is unlikely that
you will have a photoplotter to hand! The first step is to select the correct device to print to using
the Printer Setup command on the Output menu. This activates the Windows common dialogue
for printer device selection and configuration. The details are thus dependent on your particular
version of Windows and your printer driver - consult Windows and printer driver documentation
for details.
Then, with a layout loaded, invoke the Print command from the Output menu.
The dialogue forms offer a number of controls, all of which have context sensitive help
associated with them (context sensitive help on dialogue forms is accessed with a ‘point and
shoot’ mechanism via the ‘?’ key at the top right of the dialogue form). The default settings
should do for getting something and you commence output generation by clicking on OK.
Output can be aborted by pressing ESC, although there may be a short delay before everything
stops whilst Proteus and your printer/plotter empty their buffers.
With plotters in particular, you will probably need to experiment with pens, paper, and the
various settings on the Set Devices dialogue form in order to get optimum results. Full details
may be found under the chapter Hard Copy Generation in the reference manual.
The PCB Layout will remember your printer settings from the Printer Setup dialogue
and maintain them independently of your printer settings for other applications. This
means that you can configure a default set of printer options solely for use with the
Layout application.

PCB Layout
167
Output for Manufacture
The PCB Layout module provides two main output options for board manufacture:
Traditional Gerber/Excellon (available in all professional versions).
ODB++ Manufacturing Output (available in Advanced Feature Set only).
From a user interface perspective both options are very similar but from a manufacturing
perspective, the ODB++ option provides far more information than the older Gerber formats.
Examples include:
Inclusion of the connectivity information (the netlist) with the output fileset.
Explicit support for plated/unplated specification on pads.
Explicit support for fiducials.
All of this means that when viewing the output fileset from ODB++ the verification process is
simpler and more complete. However, traditional Gerber/Excellon output is still prevalent in
manufacture and would be sufficient for most purposes.
Regardless of your option the basic procedure is the same. When you invoke either of the
output options you will most likely be prompted to run a pre-production check. This runs an
automatic checklist to test for some common design errors and will report either a pass or a fail.
The Pre-production check (PPC) prompt
If your pre-production check reports errors we strongly recommend that you resolve them
before proceeding to the manufacturing output dialogue. Please also note that pre-
production check is an aid to the designer in quality assurance but not a guarantee;
manual inspection of the layout is recommended and a prototype should always be made
and tested before mass production.
More information on the Pre-production Check can be found in the CADCAM Output
section of the online reference manual (Help Menu).
Assuming a pass you will then be provided with the Manufacturing Output dialogue form.

168
The Gerber / Excellon Output dialogue form
The options in the top section of the dialogue form are self-explanatory but there are some
points of note regarding the rest of the configuration options.
The software attempts to populate the layer set with those layers used on the layout but this
should always be verified. One of the most common problems with manufacture occurs when
the manufacturer is not supplied with the full board information.
The Apply Global Guard Gap option will set the expansion of the resist plot around pads and
vias to the distance specified when this option is checked. This will take effect on all pads and
vias except those which have been manually altered on the layout. Some board manufacturers
prefer to create the resist plot in house and this option could then be used to remove any resist
expansion pre-manufacture. Unless otherwise directed we recommend that you leave this
option unchecked.
The Slotting /Routing Layer option specifies explicitly which layer of the board is to be used for
defining the routing strokes for cutouts and slots. In our case, we have used MECH1 and we
must therefore set this via the selector.

PCB Layout
169
Select the required slotting layer
The Bitmap/Font Rasterizer option controls the thickness of trace used to render bitmaps and,
more importantly, power planes. The higher the resolution the better tonality of the resulting
bitmaps but the larger the files. It is also possible that some manufacturers have a minimum
width requirement and in such cases it may be necessary to reduce the DPI settings to conform
with this. Generally speaking however, the default settings are fine.
The option at the bottom left allows you to automatically load your output into either the
Labcenter Gerber Viewer (CADCAM Output) or the Valor ODB++ Viewer (ODB++ Output). This
is useful if you want to verify the output fileset before passing to your manufacturing house.
If you intend to panelize the board you should use the Gerber X2 output in the
CADCAM Output command, then close the project, open the gerber module and
import your CADCAM files, selecting Panelization Mode from the resulting dialogue
form. Panelization is only available with Gerber X2 output - you cannot create
panels from RS274X Gerber.
Finally, the Notes tab allows us to insert any relevant information or special considerations for
the manufacturer. This is very important when we have specified a slotting layer as there is no
standard way to pass this information through. A simple note that the information on MECH1 is
for slotting will suffice.
Having configured the necessary option we can generate the files and send for manufacture.

170
APPENDIX: Creating New Packages
Library Importer
Proteus comes pre-supplied with a large quantity of footprints, and we have seen previously
how to select and place these parts on to a layout. However, it may be necessary at times to
create your own custom footprints or symbols – also a simple task with Proteus – and this
process is detailed below.
While the following topics are a detailed explanation of how to create component parts
in Proteus, in practice this should almost never be necessary. In addition to the many
installed libraries the universal part importer provides support for almost all third party
part vendors (Ultra-Librarian, Samacsys, SnapEDA, etc.). If the part doesn't exist in
Proteus itself the next step is to search for and then import it directly from a third party
vendor. This is discussed in some detail in the importer help file and shown on our
Youtube Channel.
Drawing the Footprint
In our example, we will create a SQFP44 footprint with 0.8mm pitch and 12mm width. You may
also wish to refer to the more advanced video tutorials linked below:
Finished SQFP44

PCB Layout
171
Start by selecting rectangular SMT mode. We want a pad 0.5mm by 1.8mm that should already
exist as M0.5x1.8.
The Pad used in the M0.5x1.8
If the pad style does not exist you can easily create it as discussed earlier in the
tutorial (Click on the ‘C’ button above the Object Selector).
Make sure that the Layer Selector is on Top Copper and place one of the pads in the usual way.
Right click to cancel placement immediately after placing a single pad and then left click on the
pad to highlight it. With the pad highlighted, go to the Edit Menu and select the replicate
command. Alternatively you can right click on the pad and select replicate from the resulting
context menu.
Right click and select the replicate command
The replicate command will action on tagged objects so you should ensure that you
have only the placed pad highlighted before invoking this command.
There are 11 pads on each side of the footprint so we need to replicate 10 times with an X-Step
of 0.8mm as per the following screenshot.

172
Replicate Dialogue
Note that you need to include the units of either millimetres (mm) or Thou (th) when
entering values in to the X/Y-step fields.
This will give us a single row of pads of the correct pitch (zoom in, change the snap settings and
measure if you would like to confirm). The next step is to duplicate this row of pads to form the
bottom of the footprint.
Start by right dragging a tagbox around the entire row of pads and then go to the Edit menu and
select replicate. This time we want only one copy, 12mm down (or up) from the current row. Use
negative co-ordinates if you want the duplicated row beneath the current one or positive co-
ordinates if you want it above.
We now need to repeat the process with the other two rows. Drag a tagbox around a full row,
right click inside the tagbox and select Block Copy from the resulting context menu.
Block copy will copy everything inside the tag box

PCB Layout
173
Move the mouse and drag the copy to a free area, left clicking to place and then right clicking to
exit copy mode. Now, drag a tagbox around the row, right click and select the Block Rotate
option, specifying a 90 degree rotation to align the pads correctly.
Block rotation of 90 degrees
In order to position this row of pads correctly it’s best to first set place a marker on the location
we want to move the row of pads to. For this footprint the centre of the top pad on the left hand
side is 2mm below and 2mm to the left of the centre of the left hand most pad on the top row.
This gives us enough information to accurately position the row.
Select marker mode in preparation and then move the mouse over the left hand most pad on
the top row until it is encircled. You’ll want to be on a fairly precise snap setting for this (e.g.
0.5mm or F2 shortcut key).
Make sure the pad is encircled
If you find your snap settings in thou you need to switch to Metric mode, either by hitting the ‘M’
key on the keyboard or via the Metric option on the View Menu.
Now, hit the ‘O’ key on the keyboard to set a false origin at this location and then invoke the
Goto-XY command from the View Menu.

174
Type in –2mm in both the X and the Y co-ordinate fields (i.e. down and left) and make sure that
the offset is relative to the current origin. Select OK and click the mouse twice to place the
marker at this location.
OK will take the mouse to the specified location
The marker we have placed will serve for now as the location we want to centre the top most
pad of our third row. Simply draw a tagbox around the row, left depress the mouse inside the
selection box and drag into position. You will almost certainly need to use the zoom commands
(F6, F7 or the middle mouse wheel) and possibly also adjust the snap setting (CTRL+F1) to get
accurate positioning.

PCB Layout
175
Moving the centre of a pad on to the marker
Having placed the row of pads right click on the marker and delete it – we’ll come back to
marker placement later on. The final stage of pad placement is to replicate the newly placed row
of pads onto the right hand side. As before, draw a selection box around the row of pads and
use the replicate command with an X offset of 12mm to duplicate the row.
Adding the silkscreen graphics is now straightforward. Select the 2D Graphics Line icon, make
sure the Layer Selector is on top silk and place four lines along the inside edges of the pads to
form a box. You’ll find this much easier to do if you change the snap settings upwards (e.g. F2).

176
Placing the Top Silk area
The next job we have is to number the pads. Start by invoking the Auto Name Generator from
the Tools Menu. We don’t need to enter anything in the string field here; simply leave the
defaults and click on the pads consecutively to number them, Number 1 is the top pad on the
left hand row.
Auto Name Generator

PCB Layout
177
Remember to hit the escape key on your keyboard when you have finished numbering pin 44 to
exit assignment mode.
It’s common to place a small dot beside pin one and you can do this via the 2D Graphics circle
icon. Make sure that the Layer Selector is on Top Silk and turn the snap setting down to
minimum (CTRL+F1) to achieve finer control over the size.
Place a small dot where Pin 1 is
The final step is to specify where we want the origin of the device to be (for placement
purposes) and where we want the silkscreen graphics for the package reference to appear.
Both of these are done with markers.
Select marker mode and make sure that ORIGIN marker is highlighted in the Object Selector.
You’ll recall that we used this as a reference point earlier but its real job is to specify the origin
of the component for placement and rotation. This is really a decision for the user but typically
the origin is either pin 1 or the centre of the component. For simplicity here, we will place the
origin on pin 1; left click to begin placement, move the mouse over the centre of pin 1 and left
click again to commit the origin marker.
Origin marker placed
Now, change the marker type to be REFERENCE in the Object Selector. The Reference marker
dictates where the component reference (e.g. U1, R12, C3) is placed by the software relative to
the component. Again, this is very subjective but we’ll set it above and slightly to the left of the
part.

178
Reference marker placed
Having completed the layout of the footprint, we can now move on to the (far simpler) process
of packaging the part into the libraries.
Circular Pad Placement
The replicate command is dynamic based on whether you are in cartesian co-ordinates or polar
co-ordinates (View Menu Toggle). If you needed to place pads in a circular shape you would:

PCB Layout
179
Select Polar mode (View Menu).
Place a False Origin ('O' shortcut key).
Orient your first pad and place at radius distance from (false) origin.

180
Right click on the pad, select replicate command and specify angle (e.g. 20) and number
(e.g. 17) to complete the circle.
Packaging the Footprint
Drag a selection box around the entire footprint and then select the Make Package command
from the Library Menu.
Launch 'Make Package' from the Library menu
The first screen is fairly self-explanatory and similar to that we’ve seen in the schematic capture.
Note that the package description is searchable when we are browsing for footprints so a little
effort to make this as descriptive as possible is worthwhile. You will also want to create the part
in the USERPKG library which is the default library supplied for user footprints. For our
purposes, we’ll call this package TESTPKG and give it some basic entries.

PCB Layout
181
The Make Package dialogue form
You can create your own libraries via the Library Manager – please see the
reference manual for details. You should not make your own parts into the other
pre-supplied libraries as Labcenter may overwrite these libraries during upgrade
installs.
When this is filled out, switch tabs to the 3D Visualisation tab (do not hit the OK button at this
stage – we still have some work to do). Essentially what we need to do here is provide as much
information as possible in order to get a sensible 3D image of the part which can then be used
when we use the 3D Viewer to examine a board. This job is greatly aided by a 3D Preview on
the dialogue form that will update live as we adjust parameters. Discussion of parameters and
values is beyond the scope of this tutorial and is discussed in some depth in the online
reference manual (Help Menu in the PCB Layout – Help Index). For our purposes, simply fill out
the property fields as shown in the next section.
3D Visualisation
This is where you would either provide a STEP file or use the Labcenter script to provide a
geometric model for the part. In either case, you will get a 3D representation of the part in the
3D Viewer and can then export to Solidworks or other MCAD toolchains for case and mounting
design.
If you are providing a STEP file you must:
1) Download the STEP file from the internet and place in the MCAD directory of your
Proteus installation.
2) Import via this dialogue.

182
3) Rotate and offset such that the part is aligned correctly on the 2D courtyard. Note that
you can zoom in and out on the preview with the middle mouse wheel (or buttons) and
the flip command will mirror the board at its current position.
Fortunately, this job is greatly aided by the number of STEP files available on the internet (e.g.
www.3dcontentcentral.com) and a 3D preview on the dialogue form to help with alignment.
Setting the 3D parameters
Discussion of geometric model parameters, values and importing models is beyond the scope
of this tutorial and is discussed in some depth in the online reference manual (Help Menu in
PCB Layout – Help Index). Geometric models are ideally suited to large pin count parts with
small extrusion (e.g. BGA, QFP)
STEP files, while common, are often poorly made resulting in large file sizes. Bear
in mind the bigger the STEP file the slower the 3D Viewer will render. Consider
using geometric models where no sensibly sized STEP file is available.
If you now select the Package Icon, you will see that TESTPKG has appeared in the Object
Selector, and can be placed like any of the packages you have used so far. Also, if you place
the part on the layout and invoke the 3D Visualisation engine from the Output Menu (PCB
Design Level 2 or higher required) you will see the 3D rendered image of the part.

183
VSM TUTORIAL (Interactive)
Introduction – Interactive Simulation
The purpose of this tutorial is to show you how to conduct an interactive simulation with a
microcontroller using Proteus VSM and the VSM Studio IDE. The emphasis will be on practical
usage of the simulator and IDE, with more detailed coverage of each topic being available in the
reference manuals. This tutorial does not cover schematic entry; if you are not familiar with
drawing in Proteus then you should take the time to work through the tutorial content in the
Proteus reference manual.
We will use a pre-drawn schematic of the Microchip F1 Evaluation Board as shown below.
Starting from the basics of driving the simulation from the VSM Studio IDE we will then look at
some of the various debugging and measurement tools available inside the Proteus VSM
software.

184
Requirements
To work through this tutorial you will need:
An installed copy of the Proteus Software at Version 8.0 or later. A demonstration copy of
the software can be downloaded free of charge from the Labcenter website if you do not
have a professional copy.
An installed copy of the Hi-Tech PIC16 compiler at Version 9.8 or later. Download and
installation of this compiler can be managed from within the Proteus software VSM Studio
IDE); we will cover the procedure for this later in the Project Setup section of the tutorial
below.
We would still recommend you read through the tutorial, even if you do not have the tools
installed. Most of the material - and all of the debugging techniques – are generic and will prove
useful in your own designs.
Project Setup
The first thing we need to do is setup our Proteus 8 project. Since we are using a pre-drawn
schematic in the form of a virtual development board this procedure is much simplified.
From the home page in Proteus launch the new project wizard and select the development
board option. Next, change the microcontroller family to be PIC16 and finally the F1 Evaluation
board (F1 Release) from the listbox at the bottom. Click finish to import the project.

Proteus VSM
185
After project import you should see two tabs in the application, the schematic capture module
with the F1 Evaluation Board design and the VSM Studio IDE containing the standard Microchip
source code for driving the hardware.
The first thing we need to do is compile the source code and produce some firmware that we
can test in simulation.
Compiler Configuration
The Microchip source code was written using the Hi-Tech PIC16 compiler so we need to have
this tool installed in order to compile firmware. Switch to the VSM Studio tab and launch the
compilers configuration dialogue form from the Config Menu.
The dialogue form lists all of the supported compilers along with an indication of whether or not
they are installed and configured or not. Pressing the 'Check All' button at the bottom of the
dialogue will scan your computer for compilers and - if found - will configure them to work
directly from within Proteus.
Open source compilers can be downloaded and installed directly from Labcenter's servers.
Links are provided to the download page on the vendors website for proprietary compilers. The

186
Hi-Tech compiler we need requires download from Microchip's website so if you don't have this
compiler installed you will have to:
1) Click on the goto website button beside the compiler.
2) Download and install the compiler.
3) Click on the Check All button at the bottom of the dialogue form to configure the compiler to
work with Proteus.
You should notice after running this command that the Hi-Tech compiler row on the dialogue
form is marked as installed. The output window at the bottom of the IDE will also report on the
results of the compiler checking.
At this stage we have compiler, source code and schematic all in place. Use the Build Project
command on the Build Menu in VSM Studio (or the build icon) to compile your firmware.

Proteus VSM
187
Output from the compiler is written to the bottom pane of the IDE and you should get a compiled
successfully message on completion.
The next step is to run the simulation and test our compiled code on the virtual hardware.
VSM Studio automatically configures common compiler options to correctly build
your programs for simulation in Proteus. If you need to tweak settings (e.g. link to
external library) you can do so via Project Settings on the Build Menu.
Running a Simulation
Running a simulation is as simple as pressing the play button on the animation control panel at
the bottom left of Proteus.
You should see that the schematic tab comes to the foreground and that the LCD panel
displays the default time.

188
The Microchip demonstration code for the F1 Evaluation Board has three modes, one for time,
one for temperature and a third which gives an ADC reading from the POT. You can interact
with the simulation and cycle through the modes of operation by pressing the control button on
the schematic.
When in temperature mode you can adjust the temperature on the MCP9800 temperature
sensor by clicking on the increment or decrement buttons. The current temperature is
transmitted on the I2C bus to the PIC processor and then formatted and displayed on the LCD.

Proteus VSM
189
When in voltage mode you can adjust the value of the POT. The voltage reading is converted
by the processor and then displayed on the LCD panel.
The PIC microcontroller has a 10-bit LCD so our displayed value range is 0 to 1023 over
the 0 to 3.3V range.
When you are finished press the stop button on the animation control panel to stop the
simulation.

190
Important Notes
Quite a lot is happening when we run a simulation in Proteus that might not be immediately
apparent.
Firstly, the micro-controller on the schematic is executing the compiled firmware file in exactly
the same way as a physical PIC would execute its programmed firmware. Working with the
VSM Studio IDE simply automates the 'programming' step by sending the output file to the
schematic after a successful compile.
You will have noticed that almost all of the wires on the schematic end in a terminal with a
name. For those unfamiliar with terminal connections it is worth explaining how this works. On
the schematic, any two terminals with the same name are considered connected (like a 'virtual'
wire). For example, the RC3 and RC4 terminals at the side of the temperature sensor
correspond to the RC3 and RC4 terminals connected to the I2C pins on the PIC processor.
We tend to lay out schematics like this to avoid spaghetti wiring and to split the schematic into
easily identifiable logical blocks. The important thing to understand is that all signals travel on
the visible wires. This means that you can attach a voltage probe or measurement instrument
anywhere that you can see a wire (indeed, we will do both later in the tutorial). All that Proteus
does is 'jump' the signal between the two terminal ends as though there was a single wire
connection. You can read up more on this type of connectivity in the Proteus reference manual.
Finally, the status bar at the bottom of the application reports the simulation time elapsed.
Depending on the power of your computer, the clock speed of the processor and complexity of
the schematic, a particular simulation may not run in real time but it will always run
synchronously and the execution time is reported on the status bar.
As an example, on a particularly slow computer this simulation in clock mode may not advance
as the clock on the wall advances but it will always advance as the simulation time advances.

Proteus VSM
191
Writing Firmware
Now that we have completed the workflow through simulation let's add some functionality to the
program. We know that pressing the button switches between time display, temperature and
POT display so we can easily add another mode of operation here. Start by switching to the
VSM Studio IDE tab and opening up the main.c file (double click on the item in the project tree).
You will see near the top of the file that there are some function prototypes and an enumeration
of the modes of operation. We need to add a new function prototype for our test mode and also
add a corresponding value to the enum. You can add the following:
Next, we need to find the button switching logic in order to add our new mode of operation. The
easiest way to do this is to search for one of the other modes. Right click on the editing window
in VSM Studio, select Find from the resulting context menu and then enter MODE_POT as the
search term.

192
Almost the first hit is the one we are looking for, namely a switch statement on button release
that cycles through the setting of the display modes. All we need do here is add our new mode.
Note that you need to change the display mode on the previous case statement as
well.
Just below this in the code there is another switch statement which actions the current display
mode. Again, we need to our case here and call our function.

Proteus VSM
193
The last step is to write a function that does something when we enter our mode of operation.
We'll add this at the bottom of the file.
You can experiment and add anything you like here but we'll do something simple, writing a
value to the display and adding a little binary counter on the LED's.
Since we are using PORTE to write the LED's here we also need to configure the port pins.
We'll set up ANSELE in the peripheral config section at the top of the main function.
The final step is to build the project and launch Proteus as discussed before. If you have made
a mistake (as we have here) you will get a compiler error in the output window. Clicking on this

194
error will navigate to the problem. In our case we have missed a semi-colon from the end of the
line.
Some errors - such as linker errors - will obviously not be navigable. In these cases
you may need to change the options/includes via the project settings command.
When we run the simulation this time we can use the button to cycle through the modes of
operation until our own is reached (time -> temperature -> test). We should see our displayed
number on the display at this point and a byte cycle count on the LED's
Again, press the stop button on the animation control panel to stop the simulation.
This example is a little contrived and not terribly exciting but it does show how you can quickly
write and simulate code on virtual hardware.
Active Popups
So far, we have been writing our code in the VSM Studio tab and simulating on the schematic
capture tab. There is nothing wrong with this and it can work very well on two monitors if you
drag one of the tabs onto another screen.
When debugging however, you are typically more interested in stepping the code and looking
only at small sections of the board for verification. The active popup system in Proteus is
designed to do exactly that - bringing defined sections of the schematic into VSM Studio during
simulation.
In our case, the temperature sensor is a good example of something we might want to see and
interact with during debugging. To add it as an active popup:
1) Switch to the Proteus tab and selecting the Active Popup icon.

Proteus VSM
195
2) Start at the top left and drag a box around it.
3) You should see a blue dashed line around the area when you are finished.
If you make a mistake you can right click on the dashed line and delete. Similarly, if
your positioning is wrong, you can right click on the dashed line and drag.
Other likely candidates for active popups are the mode selection button, the POT and the
display itself so we can repeat the process above, dragging additional boxes around these
items. Your schematic should look something like the following when you are finished.

196
Since we have specified active popups the assumption is that we will be working (debugging)
inside VSM Studio. If you press the play button to run the simulation now you should find that
you switch to the VSM Studio tab and that the active popups appear docked on the right hand
side of the IDE.

Proteus VSM
197
The source and variables areas of the tab will display a simulation running message
at this point as we are freely executing code. We'll cover debugging in the next
section of the tutorial.
Active popups are clever not only because they bring areas of the schematic into the debugging
environment but because you can interact with them. For example, if you click on the S1 button
to switch modes you should see the display change to the temperature on the I2C temp sensor
and if you then adjust the temperature on the sensor the display should reflect the changes.

198
You can switch back to the schematic tab and you will see exactly the same status as in the
active popups. When you stop the simulation (from the animation control panel) the active
popups will disappear and VSM Studio will switch from its 'debugging layout' to its 'design
layout' where you can once again edit and compile your source code.
You can only create or adjust active popups on the schematic when the simulation
is stopped. You can however resize active popups inside VSM Studio by dragging
while the simulation is running.
Now that we have configured our active popups we can start to look at how to debug problems
when things don't quite work the first time.
Basic Debugging
Much of the real power of Proteus VSM comes from its debugging capabilities. We have already
seen how we can write code and test during free running simulation and we'll now look at how
to step through our code in simulation time.
Start the simulation with the pause button on the animation control panel
The program will switch to the VSM Studio tab, active popups will display on the right hand side,
the main panel will report a 'no source line message' and a list of program variables will appear
at the bottom of your screen.

Proteus VSM
199
At this stage the simulation has 'booted' and a stable operating point has been found but no
instructions have executed and no real time has elapsed.
No source code is shown as there is no source line at the current program counter value
You can select any of the program source files from the combo box at the top of the window but
we will start with the main.c file which contains the principle program control loop.

200
To take a simple example, let’s set a breakpoint in the main event loop when a button is
released. The easiest way to set/toggle a breakpoint is to double click on the line of code that
you wish to break on. The breakpoint indicator should appear at the left of the source window
beside the line of code in question. If you set a breakpoint by mistake then you can remove it or
toggle it off by double clicking again on the line (or from the right hand context menu).
If we run the simulation now (play button) it will switch happily execute in free running mode
until we release the mode switch button (S1) at which point the code for button release will be
hit and the simulation will pause. You can do this easily by clicking on the button in the active
popup window.
Having hit our breakpoint we can single step our code (and the system) via the usual
commands which can be found at the top right of the source window or on the debug menu in
VSM Studio. Alternatively you can use the F10 and F11 shortcut keys for 'step over' and 'step
into' respectively.

Proteus VSM
201
If you really need to examine behaviour in detail you can even step the code at assembly level.
Right click on the source menu and select 'disassembly' from the resulting context menu and
then use the same step commands as before.
Right click and select disassembly again to return to high level source code stepping
You may notice during step debugging that the active popup for the display does
not show a full legible output. This is correct and a consequence of the display
being multiplexed.
If you want to run through to the next button release simply press the play button on the
animation control panel and then click the button on the active popup to trigger the breakpoint
again.
Right click and select clear all breakpoints when you are finished and then press the stop button
on the animation control panel to end the debugging session.
Important Notes
When you hit a breakpoint or single step debug in Proteus it is important to understand that you
have the entire system under time control. This means for example that capacitors will not
discharge or motors lose momentum when the system is paused. When you step over a
command the instructions are executed, the effect of those instructions are propagated through
the system and then the system will pause again. You can see this controlled advance of time
via the output on the status bar during debugging.
Many additional debugging windows are available which are not discussed in this tutorial. All of
these can be launched from the debug window in VSM Studio and will appear at the bottom of
the IDE. Data will be displayed on the windows whenever the simulation is paused. The watch
window - which is a special case - is discussed separately in the next section of the tutorial.
The Watch Window
The watch window is the one debugging window that provides live data during free running
simulation and it also gives us a different way to target breakpoints. To start with, let’s use the
watch window to monitor the ADC conversions from the POT.

202
Start the simulation using the play button at the bottom of Proteus and then launch the watch
window from the debug menu in VSM Studio. You should see it appear as a docked tab at the
bottom of the IDE.
Next, right click on the watch window and select 'Add items by name' from the context menu.
We want to add the ADC registers ADRESH and ADRESL which you can do by double clicking
on an entry. Exit the dialogue form when you are done and you should see both items appear in
the watch window display.
We now need to use the active popups (or switch to the schematic tab) to switch into POT
reading mode. Click on the control button three times to cycle the modes and then use the
actuator buttons at the left of the device to vary the value on the POT.

Proteus VSM
203
You can change the display format of the items to binary if you find it easier to understand the
results. You would do this by right clicking on each item in the watch window and changing the
display format to binary.
Since this is 10-bit ADC we would expect the maximum value to be 1023 or 0x03FF and we
should see this value when the POT is fully ramped up.
Now let’s assume that we needed to catch the midpoint on the way back down. We know that
the midpoint value result should be around 0x1FF so we can set conditions on the watch items
to trigger a breakpoint. We do this by right clicking on a watch item and selecting watchpoint
condition from the context menu. In our case we would want to stop when both ADRESH is
equal to 0x01 and when ADRESL is less than or equal to 0xFF. This will work as the first time
we hit this value on the way down from the maximum will be at the midpoint voltage.

204
Note that you need to separately configure ADRESH and ADRESL. The watch window display
should look like the following when you are finished.
Having set up the watch conditions all we need do now is adjust the POT back down until the
breakpoint kicks in when the conditions are met. As before you can do this either via the POT
active popup inside VSM Studio or by switching to the schematic tab. When triggered you
should see that the value on the watch items is 0x1FF and - if need be - you could start single
stepping your code at exactly the point the conditions were triggered.
Watch conditions are particularly useful for things like debugging timer code when
you want to trap an overflow condition.
You can disable watch point expressions by right clicking on a watch item, selecting
watchpoint condition and then selecting the 'turn off watchpoints' option from the
resulting dialogue.
Before we move on to discuss hardware breakpoints either disable the watchpoint conditions
(as described above) or delete the watch items completely and then press the stop button on
the animation control panel to end the simulation.

Proteus VSM
205
Hardware Breakpoints
So far, we have looked at how to break into the simulation based on software conditions
(watchpoints and breakpoints). It is also possible to use hardware breakpoint objects in order to
check the code when a hardware condition occurs. As an example, if we wanted to catch the
beginning of activity on the I2C bus we could set up a hardware breakpoint on the I2C line as
follows.
Switch to the schematic tab and then select the voltage probe icon from the mode selector on
the left hand side. Next, click on the editing window to begin placement, move the mouse over
the SDA line on the bus and left click again to drop the probe on the wire.
Now right click on the probe and select edit properties from the resulting context menu.
Select digital breakpoint and we want to trigger on active low so enter 0 as the trigger value.

206
Hit OK and then press play to run the simulation. You should find that the simulation will pause
almost immediately and the source window in VSM Studio will show that we have just executed
a command to set SDA low.
This breakpoint is actually taking place inside the initialization routine. If we wanted to skip this
and activate only when we enter I2C mode we need to set and arm time on the breakpoint. Do
this by stopping the simulation, switch to the schematic module and edit as before. Set the arm
time to 1 second.

Proteus VSM
207
This time when we run the simulation the breakpoint will not trigger until we press the mode
selection button to enter temperature mode (where temperature is transmitted on the I2C bus).
You should find that you end up inside one of the I2C routines in the source code. You can
follow the code path from here using the stepping and debugging described in previous
sections. Stop the simulation again when you are finished.
Interactive Measurements
It is quite common to want to examine signals and waveforms on the design and Proteus
provides two main ways of doing this. As an example, let's assume we need to examine the I2C
traffic from the MCP9800 temperature sensor; we can do this either interactively or by more
traditional graph based methods.
The first thing we need to do is tidy up the schematic and remove the debugging items we have
used previously. You can remove the voltage probe by right clicking on the probe on the
schematic and selecting delete from the context menu. Similarly, we can right click on the
border of the active popup objects and delete them.
When an active popup is defined on the schematic Proteus will switch to VSM
Studio when the simulation starts as it is assumed you are primarily debugging
source code. Since we are now analyzing signals we want to remove the active
popups so that the simulation starts with the schematic tab open.
The next thing to do is to get the I2C debugger placed and connected. Select the instrument
icon which produces a list of available interactive measurement tools in the parts bin. In our
case, the obvious candidate is the I2C protocol analyser.

208
Click on the I2C analyser in the parts bin to select it and then place it on the schematic in the
usual way. For ease of wiring, you'll want to drop it underneath the temperature sensor.
Next, we need to wire up the pins. Note that the cursor turns green on both a starting and
stopping point for a wire. The wiring procedure is therefore to position the mouse over the
starting point (the pin on the I2C debugger) until the cursor turns green, left click to start
placement, move mouse to destination point (cursor turns green) and finally left click to
terminate placement. Use this technique to connect both the SCL and the SDA lines to the I2C
bus.

Proteus VSM
209
Once we have wired up the analyser we can start the simulation. You should see straight away
that there is an additional window for the I2C debugger and what seems to be some
initialization/identification traffic. To view normal transmission we need to press the button on
the schematic to switch into temperature mode display.
Since the code is constantly polling you should then pause the simulation from the animation
control panel so that we can take some time to analyse the traffic.

210
If you are working within a single frame the VSM Studio tab will come to the
foreground when the simulation is paused as it is assumed you are interested in the
source code pending execution. The analyser will however remain on top. If you
want to see both the schematic and the source at the same time you can either use
Active popups or drag the VSM Studio tab onto some free space to separate it.
The syntax used in the protocol analyser is standard and should be familiar. You can expand
any sequence via the '+' box on the left hand side. The peripheral (MCP9800) has a standard
address of 0x90 so we can see from the read requests that the sequence is start (S), followed
by read request 0x91 (Read request, bit 0 set), followed by 0x1B (data) and so on. As you
would expect the data received (0x1B) is 27 decimal corresponding to the temperature currently
displayed on the peripheral.
You can experiment with this by running the simulation, changing the temperature on the
MCP9800 schematic part and then pausing again to check the display output on the I2C
debugger.

Proteus VSM
211
Do note that with constantly polling firmware such as this there is considerable overhead in
terms of performance as we are constantly writing textual data to the display. However, in most
cases you are using the instrument for testing or debugging, at which point the simulation speed
is secondary to problem solving. As with all debugging windows you can close the debugger
when not in use and then re-open it from the Debug Menu in either VSM Studio or Proteus.
Further Reading:
More information on the protocol analyser - along with other instrumentation – is available
in the Proteus VSM reference manual. In particular, note that you can use the analyser as
an I2C master (or slave) device as well as simply as a monitor.
More information on picking, placing and wiring on the schematic can be found in the
Proteus tutorial documentation, launchable from the home page.
Graph Based Measurements
We can look at the same traffic in a different way by using graph based simulation. There are
however some important differences which affect how we set up the simulation, namely:
You cannot interact with the circuit during a graph based simulation.
A graph based simulation runs for a specified period of time.
The results are not visible until this period of time has finished and the simulation has
stopped.
Given the above, let's look at how we might analyse the I2C traffic with a digital graph. First of
all, delete the interactive I2C debugger by right clicking on it and selecting delete from the
context menu.
Next, make some space for the graph by dragging a tagbox around the display and wires with
the right mouse button so that they all highlight. Left depress the mouse and drag the lot to the
right of the schematic.

212
Now select the graph icon and then the digital graph from the parts bin. Left click the mouse at
the top left of where you want the graph to be and then move the mouse down and to the right.
Left click again to commit placement.
Note that the graph on the schematic doesn't need to be particularly large. We will
maximise it later when we want to analyse the simulation results.
Having added the graph we now need to tell it which wires we want to trace. We do this by
attaching probes to the wires and then specifying the probes as traces on the graph. Select the
voltage probe icon and then place a probe on each of the two I2C lines. This is done exactly as
we discussed earlier in the section on hardware breakpoints.

Proteus VSM
213
If you need to make some room for the probes, right click on the terminal at the end of the wire,
right click and select drag object from the context menu and move to the left to make room for
the probe.
You can use the middle mouse button or the F6/F7 keys to zoom in and out around
the mouse position if you need to get in closer. The F8 key will return to the default
view of the schematic.
By default, the voltage probes will pick up the name of the terminal. It’s useful to rename them
to be more meaningful in the context of our simulation. You can do this by right clicking on the
probe, editing its properties and then changing the name to be SCL or SDA respectively.
Now that we have the probes on the wires and the graph on the schematic we need to add the
probes to the graph. There are several ways to do this but probably the easiest is simply to drag
the probe onto the graph. To do this, right click on the probe, select drag object, move the
mouse over the graph and then left click again to drop. Do this for both probes.

214
By default, a graph based simulation will run from time zero to one second of simulation time. In
our case, it would make much more sense to run from one second to two seconds, thus
skipping the initialization traffic. We can do this by editing the graph (right click and edit
properties) and changing the start and stop time.
Left clicking on an empty area of the schematic will de-select any currently selected
objects. Normally, this is done when you exit an edit properties dialogue form as the
object will still be highlighted.
We are now ready to simulate except for one significant problem. As mentioned previously, you
cannot interact with a circuit during a graph based simulation but we need to switch mode in
order to poll the temperature sensor and trigger the I2C traffic. Since we can't press the button
we need to inject an equivalent signal to the PIC so that the firmware switches into temperature
mode. We do this with generators. Select the generator icon and then the pulse generator from
the parts bin. Place the generator to the right of the button beside the RD2 terminal - you may
need to move the terminal first to make some space on the wire for the generator.

Proteus VSM
215
Now edit the generator in the usual way (right click - edit properties). Select single pulse from
the digital generator types and change the pulse polarity to be negative so that the pulse signal
represents a button push. Since we are simulating from 1s to 2s set the start time to 1.25s and
the pulse width to something like 50ms.

216
We can now run the simulation. Unlike an interactive simulation the animation control panel is
now used (we are simulating for a fixed time which does not necessarily start at time zero).
Instead, use the 'Simulate Graph' command on the graph menu. You should then see results
which look like those below.
Aside from the fact that the traffic didn't start until around 1.25s (as specified by the pulse) we
can't see much information here. Right click on the graph and select maximise from the context
menu to launch the program in a new tab.

Proteus VSM
217
When the graph tab is in the foreground the menu's and icons change to show things we can do
with the graph. In particular, notice the new graph toolbar at the top of the application
The zoom commands can be found here and probably the most useful of these is the 'zoom to
area' icon. Click on this icon and then drag around a small area to localise the display. If you
repeat this you will soon be able to zoom in on a single I2C sequence.
Alternatively, you can hold the SHIFT button down and drag a box with the mouse
to zoom into the area inside the box.
Those familiar with the I2C protocol can then verify the raw data on the graph against the
sequencing we saw earlier on the protocol analyser.
Finally, you can take measurements with the graph as follows:
Left clicking the mouse on the graph window will place a (green) cursor on the graph.
Left dragging the mouse will allows you to position the cursor
Holding the CTRL key down and left clicking will place a (red) cursor.
Left dragging the mouse with the CTRL key down will allow you to position the (red)
cursor.
Data for each cursor and delta between them is shown on the display at the bottom of the
graph window.

218
Further Reading
All of the general placement and editing techniques discussed briefly here are covered in
far more detail in the Proteus tutorial documentation.
More information on Graphing is provided later in this documentation and a full discussion
of generators, probes and graph based simulation can be found in the Proteus VSM
reference manual.
Diagnostic Messaging
Another - often overlooked - tool provided in Proteus is diagnostic messaging. This is an
interface that allows you to ask the system for a plain text report of activity in a particular
peripheral or peripherals. To look at this we will turn on diagnostic messaging for the LCD
panel.
Switch to the schematic tab and then launch the configure diagnostics command from the
Debug menu.

Proteus VSM
219
Expand the entry for the display panel, click on the entry and then change the trace information
level to full trace.
Now expand the PIC16 and scroll down to the LCD module entry, again changing the trace
information level to 'full trace'.

220
Start an interactive simulation from the animation control panel and then click on the simulation
advisor to view the diagnostic messages. This will switch Proteus to the VSM Studio tab and the
simulation advisor will appear as a docked window at the bottom of the frame.
If you pause the simulation note that the LCD messages contain PC values which you can click
on to locate the instruction in your source code that caused the condition.

Proteus VSM
221
Navigation to source code is only possible when the simulation is paused.
Finally, stop the simulation and turn off diagnostics in the same as they were enabled, except
change the trace information levels back to warnings only.
Diagnostic messages are particularly useful in a problem situation where you need to gather
information before deciding where to hunt for the bug. It does generate a major performance hit
try it with the PIC MSSP peripheral and MCP9800 in temperature mode for example) and
should therefore only be enabled when required. You can also choose to log over only a limited
time period if you know when the activity band of interest is.

222

223
VSM TUTORIAL (Graphs)
The purpose of this tutorial is to show you, by use of a simple amplifier circuit, how to perform a
graph based simulation using Proteus VSM. It takes you, in a step-by-step fashion, through:
Placing graphs, probes and generators.
Performing the actual simulation.
Using graphs to display results and take measurements.
A survey of the some of the analysis types that are available.
The tutorial does not cover the use of Proteus in its general sense - that is, procedures for
placing components, wiring them up, tagging objects, etc. This is covered to some extent in the
Interactive Simulation Tutorial and in much greater detail within the Proteus manual itself. If you
have not already made yourself familiar with the use of Proteus then you must do so before
attempting this tutorial.
We do strongly urge you to work right the way through this tutorial before you attempt to do your
own graph based simulations: gaining a grasp of the concepts will make it much easier to
absorb the material in the reference chapters and will save much time and frustration in the long
term.
Getting Started
The circuit we are going to simulate is an audio amplifier based on a 741 op-amp, as shown
below. It shows the 741 in an unusual configuration, running from a single 5 volt supply. The
feedback resistors, R3 and R4, set the gain of the stage to be about 10. The input bias
components, R1, R2 and C1, set a false ground reference at the non-inverting input which is
decoupled from the signal input.
As is normally the case, we shall perform a transient analysis on the circuit. This form of
analysis is the most useful, giving a large amount of information about the circuit. Having
completed the description of simulation with transient analysis, the other forms of analysis will
be contrasted.

224
If you want, you can draw the circuit yourself, or you can load a ready made design file by File
Menu ->Open Sample -> Tutorials -> Analogue Simulation Tutorial (Part 1) within your Proteus
installation. Whatever you choose, at this point ensure you have Proteus running and the circuit
drawn
Generators
To test the circuit, we need to provide it with a suitable input. We shall use a voltage source with
a square wave output for our test signal. A generator object will be used to generate the
required signal.
Click on the Generator icon: the Object Selector displays a list of the available generator types.
For our simulation, we want a Pulse generator. Select the Pulse type, move the mouse over to
the edit window, to the right of the IN terminal, and click left on the wire to place the generator.

Proteus VSM
225
Generator objects are like most other objects in Proteus; the same procedures for previewing
and orienting the generator before placement and editing, moving, re-orienting or deleting the
object after placement apply (see Generators and Probes in the reference manual).
As well as being dropped onto an existing wire, as we just did, generators may be placed on the
sheet, and wired up in the normal manner. If you drag a generator off a wire, then Proteus
assumes you want to detach it, and does not drag the wire along with it, as it would do for
components.
Notice how the generator is automatically assigned a reference - the terminal name IN.
Whenever a generator is wired up to an object (or placed directly on an existing wire) it is
assigned the name of the net to which it is connected. If the net does not have a name, then the
name of the nearest component pin is used by default.
Finally, we must edit the generator to define the pulse shape that we want. To edit the
generator, right click on it and select Edit Properties from the resulting context menu. Select the
High Voltage field and set the value to 10mV. Also set the pulse width to 0.5s.

226
Select the OK button to accept the changes.
For this circuit only one generator is needed, but there is no limit on the number
which may be placed.
Probes
Having defined the input to our circuit using a generator, we must now place probes at the
points we wish to monitor. We are obviously interested in the output, and the input after it has
been biased is also a useful point to probe. If needs be, more probes can always be added at
key points and the simulation repeated.
To place a probe, click left on the Voltage Probe icon (ensure you have not selected a current
probe by accident - we shall come to these later). Probes can be placed onto wires, or placed
and then wired, in the same manner as generators. Move the mouse over to the edit window, to
the left of U1 pin 3, and click left to place the probe on the wire joining pin 3 to R1 and R2. Be
sure to place the probe on the wire, as it cannot be placed on the pin itself. Notice the name it
acquires is the name of the nearest device to which it is connected, with the pin name in
brackets. Now place the second probe by clicking left just to the left of the OUT terminal, on the
wire between the junction dot and the terminal pin.

Proteus VSM
227
Probe objects are like generators and most other objects in Proteus; the same procedures for
previewing and orienting the probe before placement, and editing, moving, re-orienting or
deleting the probe after placement apply (refer to the section on Probes in the reference manual
for more information). Probes may be edited in order to change their reference labels. The
names assigned by default are fine in our case, but a useful tip when tagging probes is to aim
for the tip of the probe, not the body or reference label.
Now that we have set up the circuit ready for simulation, we need to place a graph to display the
results on.
Graphs
Graphs play an important part in simulation: they not only act as a display medium for results
but actually define what simulations are carried out. By placing one or more graphs and
indicating what sort of data you expect to see on the graph (digital, voltage, impedance, etc.)
Proteus knows what type or types of simulations to perform and which parts of a circuit need to
be included in the simulation. For a transient analysis we need an Analogue type graph. It is
termed analogue rather than transient in order to distinguish it from the Digital graph type, which
is used to display results from a digital analysis, which is really a specialised form of transient
analysis. Both can be displayed against the same time axis using a Mixed graph.
To place a graph, first select the Graph icon: the Object Selector displays a list of the available
graph types. Select the Analogue type, move the mouse over to the edit window, click once to
start placement, drag out a rectangle of the appropriate size and click a second time to place
the graph.
Graphs behave like most objects in Proteus, though they do have a few subtleties. We will
cover the features pertinent to the tutorial as they occur, but the reference chapter on graphs is
well worth a read. You can tag a graph in the usual way with the left mouse button, and then
(using the left mouse button) drag one of the handles, or the graph as a whole, about to resize
and/or reposition the graph.

228
We now need to add our generator and probes on to the graph. Each generator has a probe
associated with it, so there is no need to place probes directly on generators to see the input
wave forms. There are three ways of adding probes and generators to graphs:
The first method is to tag a probe/generator and drag it over the graph and release it - exactly
as if we were repositioning the object, repeat for each probe/generator. Proteus detects that you
are trying to place the probe/generator over the graph, restores the probe/generator to its
original position, and adds a trace to the graph with the same reference as that of the
probe/generator. Traces may be associated with the left or right axes in an analogue graph, and
probes/generators will add to the axis nearest the side they were dropped. Regardless of where
you drop the probe/generator, the new trace is always added at the bottom of any existing
traces.
The second and third method of adding probes/generators to a graph both use the Add Trace
command on the graph menu; this command always adds probes to the current graph (when
there is more than one graph, the current graph is the one currently selected on the Graph
menu).
If the Add Trace command is invoked without any tagged probes or generators, then the Add
Transient Trace dialogue form is displayed, and a probe can be selected from a list of all probes
in the design (including probes on other schematic sheets).
If there are tagged probes/generators, invoking the Add Trace command causes you to be
prompted to Quick Add the tagged probes to the current graph; selecting the 'Cancel' option
invokes the Add Transient Trace dialogue form as previously described. Selecting the 'OK'
option adds all tagged probes/generators to the current graph in alphabetical order.

Proteus VSM
229
We will Quick Add our probes and the generator to the graph. Either tag the probes and
generators individually, or, more quickly, drag a tag box around the entire circuit - the Quick Add
feature will ignore all tagged objects other than probes and generators. Select the Add Trace
option from the Graph menu and answer Yes to the prompt. The traces will appear on the graph
(because there is only one graph, and it was the last used, it is deemed to be the current
graph). At the moment, the traces consist of a name (on the left of the axis), and an empty data
area (the main body of the graph). If the traces do not appear on the graph, then it is probably
too small for Proteus to draw them in. Resize the graph, by tagging it and dragging a corner, to
make it sufficiently big.
As it happens, our traces (having been placed in alphabetical order) have appeared in a
reasonable order. We can however, shuffle the traces about. To do this, ensure the graph is not
tagged, and click left over the name of a trace you want to move or edit. The trace is highlighted
to show that it is tagged. You can now use the left mouse button to drag the trace up or down or
to edit the trace (by clicking left without moving the mouse) and the right button to delete the
trace (i.e. remove it from the graph). To untag all traces, click the left mouse button anywhere
over the graph, but not over a trace label (this would tag or delete the trace).

230
There is one final piece of setting-up to be done before we start the simulation, and this is to set
the simulation run time. Proteus will simulate the circuit according to the end time on the x-scale
of the graph, and for a new graph, this defaults to one second. For our purposes, we want the
input square wave to be of fairly high audio frequency, say about 10kHz. This needs a total
period of 100ms. Tag the graph and click left on it to bring up its Edit Transient Graph dialogue
form. This form has fields that allow you to title the graph, specify its simulation start and stop
times (these correspond to the left and right most values of the x axis), label the left and right
axes (these are not displayed on Digital graphs) and also specifies general properties for the
simulation run. All we need to change is the stop time from 1.00 down to 100u (you can literally
type in 100u - Proteus will covert this to 100E-6) and select OK.
The design is now ready for simulation. At this point, it is probably worthwhile loading our
version of the design (Open Sample -> Tutorials -> Analogue Simulation Tutorial (Part 2)) to
avoid any problems during the actual simulation and subsequent sections. Alternatively, you
may wish to continue with the circuit you have entered yourself, and only load the default file if
problems arise.

Proteus VSM
231
Simulation
To simulate the circuit, all you need do is invoke the Simulate command on the Graph menu (or
use its keyboard short-cut: the space bar). The Simulate command causes the circuit to be
simulated and the current graph (the one marked on the Graph menu) to be updated with the
simulation results.
Do this now. The status bar indicates how far the simulation process has reached. When the
simulation is complete, the graph is redrawn with the new data. For the current release of
Proteus and simulator kernels, the start time of a graph is ignored - simulation always starts at
time zero and runs until the stop time is reached or until the simulator reaches a quiescent
state. You can abort a simulation mid-way through by pressing the ESC key.
A simulation log is maintained for the last simulation performed. You can view this log by
clicking on the simulation advisor at the bottom left of the schematic frame. The simulation log
of an analogue simulation rarely makes for exciting reading, unless warnings or errors were
reported, in which case it is where you will find details of exactly what went wrong. In some
cases, however, the simulation log provides useful information that is not easily available from
the graph traces.

232
So the first simulation is complete. Looking at the traces on the graph, it’s hard to see any
detail. To check that the circuit is working as expected, we need to take some measurements.
Taking Measurements
A graph sitting on the schematic, alongside a circuit, is referred to as being minimised. To take
timing measurements we must first maximise the graph. To do this, right click on the graph and
select the maximise option from the resulting context menu.
This will open the graph in a new tab and change the menus and icons to include functionality
applicable to the graph.
On the left side of the screen is an area in which the trace labels are displayed and to right of
this are the traces themselves. When cursors are placed the data and delta values are
displayed at the bottom of the graph. As this is a new graph, and we have not yet taken any
measurements, there are no cursors visible on the graph, and the status bar simply displays a
title message.
The traces are colour coded, to match their respective labels. The OUT and U1(POS IP) traces
are clustered at the top of the display, whilst the IN trace lies along the bottom. To see the
traces in more detail, we need to separate the IN trace from the other two. This can be achieved
by using the left mouse button to drag the trace label to the right-hand side of the screen. This
causes the right y-axis to appear, which is scaled separately from the left. The IN trace now
seems much larger, but this is because Proteus has chosen a finer scaling for the right axis
than the left. To clarify the graph, it is perhaps best to remove the IN trace altogether, as the
U1(POS IP) is just as useful. Click right on the IN label and select Delete Trace. The graph now
reverts to a single, left hand side, y-axis.

Proteus VSM
233
We shall measure two quantities:
The voltage gain of the circuit.
The approximate fall time of the output.
These measurements are taken using the Cursors.
Each graph has two cursors, referred to as the Reference and Primary cursors. The reference
cursor is displayed in red, and the primary in green. A cursor is always 'locked' to a trace, the
trace a cursor is locked to being indicated by a small 'X' which 'rides' the waveform. A small
mark on both the x- and y-axes will follow the position of the 'X' as it moves in order to facilitate
accurate reading of the axes. If moved using the keyboard, a cursor will move to the next small
division in the x-axis.
Let us start by placing the Reference cursor. The same keys/actions are used to access both
the Reference and Primary cursors. Which is actually affected is selected by use of the CTRL
key on the keyboard; the Reference cursor, as it is the least used of the two, is always
accessed with the CTRL key (on the keyboard) pressed down. To place a cursor, all you need
to do is point at the trace data (not the trace label - this is used for another purpose) you want to
lock the cursor to, and click left. If the CTRL key is down, you will place (or move) the Reference
cursor; if the CTRL key is not down, then you will place (or move) the Primary cursor. Whilst the
mouse button (and the CTRL key for the Reference cursor) is held down, you can drag the
cursor about. So, hold down (and keep down) the CTRL key, move the mouse pointer to the
right hand side of the graph, above both traces, and press the left mouse button. The red
Reference cursor appears. Drag the cursor (still with the CTRL key down) to about 70u or 80u

234
on the x-axis. The title on the status bar is removed, and will now display the cursor time (in red,
at the left) and the cursor voltage along with the name of the trace in question (at the right). It is
the U1(POS IP) trace that we want.
You can move a cursor in the X direction using the left and right cursor keys, and you can lock a
cursor to the previous or next trace using the up and down cursor keys. The LEFT and RIGHT
keys move the cursor to the left or right limits of the x-axis respectively. With the control key still
down, try pressing the left and right arrow keys on the keyboard to move the Reference cursor
along small divisions on the time axis.
Now place the Primary cursor on the OUT trace between 20u and 30u. The procedure is exactly
the same as for the Reference cursor, above, except that you do not need to hold the CTRL key
down. The time and the voltage (in green) for the primary cursor are now added to the status
bar.
Also displayed are the differences in both time and voltage between the positions of the two
cursors. The voltage difference should be a fraction under 100mV. The input pulse was 10mV
high, so the amplifier has a voltage gain of 10. Note that the value is positive because the
Primary cursor is above the Reference cursor - in delta read-outs the value is Primary minus
Reference.
We can also measure the fall time using the relative time value by positioning the cursors either
side of the falling edge of the output pulse. This may be done either by dragging with the
mouse, or by using the cursor keys (don't forget the CTRL key for the Reference cursor). The
Primary cursor should be just to the right of the curve, as it straightens out, and the Reference

Proteus VSM
235
cursor should be at the corner at the start of the falling edge. You should find that the falling
edge is a little under 10m.
Using Current Probes
Now that we have finished with our measurements, we can return to the circuit – just close the
maximised graph for the cross at the right of the tab.
We shall now use a current probe to examine the current flow around the feedback path, by
measuring the current into R4.
Current probes are used in a similar manner to voltage probes, but with one important
difference. A current probe needs to have a direction associated with it. Current probes work by
effectively breaking a wire, and inserting themselves in the gap, so they need to know which
way round to go. This is done simply by the way they are placed. In the default orientation
(leaning to the right) a current probe measures current flow in a horizontal wire from left to right.
To measure current flow in a vertical wire, the probe needs to be rotated through 90° or 270°.
Placing a probe at the wrong angle is an error, that will be reported when the simulation is
executed. If in doubt, look at the arrow in the symbol. This points in the direction of current
flow.
Select a current probe by clicking on the Current Probe icon. Click left on the clockwise Rotation
icon such that the arrow points downwards. Then place the probe on the vertical wire between
the right hand side of R4 and U1 pin 6.
Add the probe to the right hand side of the graph by tagging and dragging onto the right hand
side of the minimised graph. The right side is a good choice for current probes because they are
normally on a scale several orders of magnitude different than the voltage probes, so a
separate axis is needed to display them in detail.

236
At the moment no trace is drawn for the current probe. Press the space bar to re-simulate the
graph, and the trace appears.
Even from the minimised graph, we can see that the current in the feedback loop follows closely
the wave form at the output, as you would expect for an op-amp. The current changes between
10mA and 0 at the high and low parts of the trace respectively. If you wish, the graph may be
maximised to examine the trace more closely.
Frequency Analysis
As well as transient analysis, there are several other analysis types available in analogue circuit
simulation. They are all used in much the same way, with graphs, probes and generators, but
they are all different variations on this theme. The next type of analysis that we shall consider is
Frequency analysis. In frequency analysis, the x-axis becomes frequency (on a logarithmic
scale), and both magnitude and phase of probed points may be displayed on the y-axes.
To perform a frequency analysis a Frequency graph is required. Click left on the Graph icon, to
re-display the list of graph types in the object selector, and click on the Frequency graph type.
Then place a graph on the schematic as before, dragging a box with the left mouse button.
There is no need to remove the existing transient graph, but you may wish to do so in order to
create some more space (right click and delete object from the resulting context menu).

Proteus VSM
237
Now to add the probes. We shall add both the voltage probes, OUT and U1(POS IP). In a
frequency graph, the two y-axes (left and right) have special meanings. The left y-axis is used to
display the magnitude of the probed signal, and the right y-axis the phase. In order to see both,
we must add the probes to both sides of the graph. Tag and drag the OUT probe onto the left of
the graph, then again drag the robe onto the right. Each trace has a separate colour as normal,
but they both have the same name. Now tag and drag the U1(POS IP) probe onto the left side
of the graph only.
Magnitude and phase values must both be specified with respect to some reference quantity. In
Proteus this is done by specifying a Reference Generator. A reference generator always has an
output of 0dB (1 volt) at 0°. Any existing generator may be specified as the reference generator.
All of the other generators in the circuit are ignored in a frequency analysis. To specify the IN
generator as the reference in our circuit, simply tag and drag it onto the graph, as if you were
adding it as a probe. Proteus assumes that, because it is a generator, you are adding it as the
reference generator, and prints a message on status line confirming this. Make sure you have
done this, or the simulation will not work correctly.

238
There is no need to edit the graph properties, as the frequency range chosen by default is fine
for our purposes. However, if you do so (right click on the graph and select Edit properties), you
will see that the Edit Frequency Graph dialogue form is slightly different from the transient case.
There is no need to label the axes, as their purpose is fixed, and there is a check box which
enables the display of magnitude plots in dB or normal units. This option is best left set to dB,
as the absolute values displayed otherwise will not be the actual values present in the circuit.

Proteus VSM
239
Now start the simulation by right clicking on the graph and selecting the simulate option from the
context menu. When it has finished, maximise the graph by opening it in a new tab as before
(right click context menu).
Considering first the OUT magnitude trace, we can see the pass-band gain is just over 20dB (as
expected), and the useable frequency range is about 50Hz to 20kHz. The cursors work in
exactly the same manner as before - you may like to use the cursors to verify the above
statement.

240
The OUT phase trace shows the expected phase distortion at the extremes of the response,
dropping to -90° just off the right of the graph, at the unity gain frequency. The high-pass filter
effect of the input bias circuitry can be clearly seen if the U1(POS IP) magnitude trace is
examined. Notice that the x-axis scale is logarithmic, and to read values from the axis it is best
to use the cursors.
Swept Variable Analysis
It is possible with Proteus to see how the circuit is affected by changing some of the circuit
parameters. There are two analysis types that enable you to do this – the DC Sweep and the
AC Sweep. A DC Sweep graph displays a series of operating point values against the swept
variable, while an AC Sweep graph displays a series of single point frequency analysis values,
in magnitude and phase form like the Frequency graph.
As these forms of analysis are similar, we shall consider just one - a DC Sweep. The input bias
resistors, R1 and R2, are affected by the small current that flows into U1. To see how altering
the value of both of these resistors affects the bias point, a DC Sweep is used.

Proteus VSM
241
To begin with place a DC Sweep graph on an unused space on the schematic. Then tag the
U1(POS IP) probe and drag it onto the left of the graph. We need to set the sweep value, and
this is done by editing the graph (right click - edit properties). The Edit DC Sweep Graph
dialogue form includes fields to set the swept variable name, its start and ending values, and
the number of steps taken in the sweep. We want to sweep the resistor values across a range
of say 100kW to 5MW, so set the Start field to 100k and the Stop field to 5M. Click on OK to
accept the changes.
Of course, the resistors R1 and R2 need to be altered to make them swept, rather than the fixed
values they already are. To do this, double left click on R1 to edit it, and alter the Value field
from 470k to X. Note that the swept variable in the graph dialogue form was left at X as well.
Click on OK, and repeat the editing on R2 to set its value to X.

242
Now you can simulate the graph by right clicking on it and selecting the simulate option. Then,
by maximising the graph, you can see that the bias level reduces as the resistance of the bias
chain increases. By 5MW it is significantly altered.
Of course, altering these resistors will also have an effect on the frequency response. We could
have done an AC Sweep analysis at say 50Hz in order to see the effect on low frequencies.
Noise Analysis
The final form of analysis available is Noise analysis. In this form of analysis the simulator will
consider the amount of thermal noise that each component will generate. All these noise
contributions are then summed (having been squared) at each probed point in the circuit. The
results are plotted against the noise bandwidth.
There are some important peculiarities to noise analysis:
The simulation time is directly proportional to the number of voltage probes (and
generators) in the circuit, since each one will be considered.
Current probes have no meaning in noise analysis, and are ignored.
A great deal of information is presented in the simulation log file.
PROSPICE computes both input and output noise. To do the former, an input reference
must be defined - this is done by dragging a generator onto the graph, as with a
frequency reference. The input noise plot then shows the equivalent noise at the input for
each output point probed.
To perform a noise analysis on our circuit, we must first restore R1 and R2 back to 470kW. Do
this now. Then select a Noise graph type, and place a new graph on an unused area of the

Proteus VSM
243
schematic. It is really only output noise we are interested in, so tag the OUT voltage probe and
drag it onto the graph. As before, the default values for the simulation are fine for our needs, but
you need to set the input reference to the input generator IN. The Edit Noise Graph dialogue
form has the check box for displaying the results in dBs. If you use this option, then be aware
that 0dB is considered to be 1 volt r.m.s. Click on Cancel to close the dialogue form.
Simulate the graph as before. When the graph is maximised, you can see that the values that
result from this form of analysis are typically extremely small (pV in our case) as you might
expect from a noise analysis of this type. But how do you track down sources of noise in your
circuit? The answer lies in the simulation log. View the simulation log now, by clicking on the
simulation advisor at the bottom of the schematic frame.
Use the down arrow icon to move down past the operating point printout, and you should see a
line of text that starts
'Total Noise Contributions at ...'

244
This lists the individual noise contributions (across the entire frequency range) of each circuit
element that produces noise. Most of the elements are in fact inside the op-amp, and are
prefixed with U1_. If you select the Log Spectral Contributions option on the Edit Noise Graph
dialogue form, then you will get even more log data, showing the contribution of each
component at each spot frequency.

Tutorials proteus schematic

More Related Content

What's hot (20)

Similar to Tutorials proteus schematic (20)

More from LITS IT Ltd,LASRC.SPACE,SAWDAGOR BD,FREELANCE BD,iREV,BD LAW ACADEMY,SMART AVI,HEA,HFSAC LTD. (20)

Recently uploaded (20)

Tutorials proteus schematic