Protel 99 se_traning_manual_pcb_design

Protel 99 SE
Training Manual

PCB Design

Software, documentation and related materials:
Copyright © 2001 Protel International Limited.

All rights reserved. Unauthorized duplication of the software, manual or related
materials by any means, mechanical or electronic, including translation into
another language, except for brief excerpts in published reviews, is prohibited
without the express written permissions of Protel International Limited.
Unauthorized duplication of this work may also be prohibited by local statute.
Violators may be subject to both criminal and civil penalties, including fines
and/or imprisonment.

Protel and the Protel logo are registered trademarks of Protel International
Limited. Design Explorer, SmartDoc, SmartTool, and SmartTeam and their
logos are trademarks of Protel International Limited.
Microsoft, Microsoft Windows and Microsoft Access are registered trademarks
of Microsoft Corporation. Orcad, Orcad Capture, Orcad Layout and
SPECCTRA are registered trademarks of Cadence Design Systems Inc.
AutoCAD is a registered trademark of AutoDesk Inc. HP-GL is a registered
trademark of Hewlett Packard Corporation. PostScript is a registered trademark
of Adobe Systems, Inc. All other brand or product names are trademarks of
their respective owners.

Contents
1 PCB Design Process .................................................................................................... 1
2 The PCB Editor Workspace......................................................................................... 2
2.1 PCB Editor Panel ..................................................................................................... 2
2.1.1 Browse Section ................................................................................................ 2
2.1.2 MiniViewer ...................................................................................................... 2
2.1.3 Current Layer Section ...................................................................................... 3
2.2 Using the Panel to Browse ....................................................................................... 3
2.2.1 Browsing Nets.................................................................................................. 3
2.2.2 Browsing Components..................................................................................... 4
2.2.3 Browsing Libraries........................................................................................... 5
2.2.4 Browsing Net Classes ...................................................................................... 6
2.2.5 Browsing Component Classes ......................................................................... 7
2.2.6 Browsing Design Rule Violations.................................................................... 8
2.2.7 Browsing Design Rules.................................................................................... 9
2.2.8 Exercises – Using the MiniViewer .................................................................. 9
2.3 Preferences Dialog Box ......................................................................................... 10
2.3.1 Options Tab.................................................................................................... 10
2.3.2 Display Tab .................................................................................................... 13
2.3.3 Colours Tab.................................................................................................... 15
2.3.4 Show/Hide Tab .............................................................................................. 16
2.3.5 Default Primitives Tab................................................................................... 17
2.3.6 Signal Integrity Tab........................................................................................ 18
2.3.7 Exercises – Exploring the Preferences........................................................... 19
2.4 Document Options Dialog Box.............................................................................. 20
2.4.1 Layers Tab...................................................................................................... 20
2.4.2 Options Tab.................................................................................................... 21
2.5 The PCB Coordinate System ................................................................................. 21
2.6 Grids....................................................................................................................... 22
2.6.1 Snap Grid ....................................................................................................... 22
2.6.2 Visible Grid.................................................................................................... 22
2.6.3 Electrical Grid................................................................................................ 22
2.6.4 Component Grid............................................................................................. 22
2.7 Shortcut Keys for Setup Options ........................................................................... 23
2.7.1 Exercises – Exploring the Document Options ............................................... 23
3 Creating a New PCB .................................................................................................. 24
3.1 Printed Circuit Board Wizard ................................................................................ 24
4 Transferring Design Information to the PCB............................................................. 25
4.1 Design Synchronization ......................................................................................... 25
4.2 Resolving Synchronization Errors ......................................................................... 26
4.3 Summary ................................................................................................................ 27
4.4 Cross Reference File .............................................................................................. 27
4.5 Design Transfer Using a Netlist............................................................................. 28
4.5.1 Loading a Netlist............................................................................................ 28
4.5.2 Resolving Netlist Loading Errors .................................................................. 29

PCB Design Training Manual i

4.5.3 Cross Reference File...................................................................................... 30
4.5.4 Editing Netlist Macros ................................................................................... 30
4.5.5 Executing the Netlist Loading ....................................................................... 30
5 Setting up the PCB Layers ......................................................................................... 31
5.1 Layer Definitions ................................................................................................... 31
5.2 Layer Stack Manager ............................................................................................. 34
5.3 Defining Mechanical Layers .................................................................................. 36
5.4 Internal Power Planes ............................................................................................ 37
5.4.1 Defining an Internal Power Plane .................................................................. 37
5.4.2 Defining a Split Power Plane......................................................................... 37
5.4.3 Moving and Editing Split Plane Vertices ...................................................... 38
5.4.4 Deleting a Split Plane .................................................................................... 38
5.4.5 Exercises – Setting up the PCB Layers.......................................................... 39
6 Setting Up Design Rules............................................................................................ 40
6.1 Adding Design Rules ............................................................................................. 40
6.2 Object Set............................................................................................................... 41
6.3 Rule Type............................................................................................................... 41
6.4 Scope...................................................................................................................... 41
6.5 Precedence ............................................................................................................. 42
6.6 Where Rules Apply................................................................................................ 43
6.6.1 Routing Rules ................................................................................................ 43
6.6.2 Manufacturing Rules...................................................................................... 43
6.6.3 High Speed Rules .......................................................................................... 44
6.6.4 Placement Rules............................................................................................. 44
6.6.5 Signal Integrity Rules .................................................................................... 44
6.6.6 Other Design Rules........................................................................................ 44
6.7 Additional Information on Rules ........................................................................... 45
6.8 Object Classes........................................................................................................ 46
6.8.1 Defining Classes ............................................................................................ 46
6.8.2 Component Class Generator .......................................................................... 47
6.9 From To’s .............................................................................................................. 48
7 Component Placement Tools..................................................................................... 49
7.1 Placing Components With Predetermined Locations ............................................ 49
7.2 Moving Components ............................................................................................. 49
7.3 Component Unions ................................................................................................ 49
7.4 Rooms .................................................................................................................... 50
7.5 Component Placement Grids ................................................................................. 50
7.6 Density Map........................................................................................................... 50
7.7 Interactive Placement Commands ......................................................................... 51
7.7.1 Alignment Commands ................................................................................... 51
7.7.2 Arrange Commands ....................................................................................... 51
7.7.3 Move To Grid ................................................................................................ 51
7.8 Auto Placement...................................................................................................... 51
7.8.1 Cluster Placer................................................................................................. 52
7.8.2 Statistical Placer............................................................................................. 52
7.8.3 Shove ............................................................................................................. 53

ii PCB Design Training Manual

7.9 Re-Annotation........................................................................................................ 54
8 Routing....................................................................................................................... 55
8.1 Interactive Routing................................................................................................. 55
8.1.1 Managing Connectivity.................................................................................. 55
8.1.2 Track Width ................................................................................................... 55
8.1.3 Interactive Routing Mode .............................................................................. 55
8.1.4 Look Ahead Routing...................................................................................... 55
8.1.5 Interactive Routing Properties ....................................................................... 55
8.1.6 Loop Removal................................................................................................ 56
8.2 Automatic Routing................................................................................................. 57
8.2.1 Automatic Routing Tips................................................................................. 57
8.2.2 Setting Up the Automatic Router................................................................... 57
8.2.3 Autorouter Options ........................................................................................ 58
9 Polygons..................................................................................................................... 59
9.1 Placing a Polygon................................................................................................... 59
9.2 Editing a Polygon................................................................................................... 60
9.3 Moving a Polygon.................................................................................................. 61
9.4 Editing Polygon Vertices ....................................................................................... 61
9.5 Deleting a Polygon................................................................................................. 61
9.6 Exercises – Working with Polygons ...................................................................... 61
10 Design Rule Checking ............................................................................................... 62
10.1 On-Line DRC..................................................................................................... 62
10.2 Design Rules Check Report ............................................................................... 63
10.3 Locating Design Rule Violations ....................................................................... 63
10.4 Exercise.............................................................................................................. 64
11 Printing....................................................................................................................... 65
11.1 Running Print/Preview....................................................................................... 65
11.2 Setting Scale and Orientation and Printer Options ............................................ 68
11.3 Copying Print Preview to the Window Clipboard ............................................. 68
11.4 PPC Documents ................................................................................................. 68
12 CAM Manager ........................................................................................................... 69
12.1 Bill Of Materials ................................................................................................ 71
12.2 DRC ................................................................................................................... 71
12.3 Gerber ................................................................................................................ 72
12.4 NC Drill ............................................................................................................. 72
12.5 Pick and Place .................................................................................................... 73
12.6 Test Point Report ............................................................................................... 73
13 3D Viewer.................................................................................................................. 74
14 PCB Library Editor .................................................................................................... 76
14.1 The PCB Library Workspace ............................................................................. 76
14.2 PCB Library Editor Panel .................................................................................. 77
14.3 Creating a Component Using the Component Wizard ...................................... 78
14.4 Manually Creating a Component ....................................................................... 78
14.5 Copying a Component ....................................................................................... 78

PCB Design Training Manual iii

14.6 Special Strings in the Library Editor ................................................................. 78
14.7 Component Rule Check..................................................................................... 79
14.8 Exercise – Libraries and Components ............................................................... 79
15 Short Cut Key Summary............................................................................................ 80

iv PCB Design Training Manual

1 PCB Design Process

Draw Schematic Annotate ERC

Create Schematic Synchroniser
Symbols (if not in
Library)

Update
Errors UpdatePCB
Schematic

Create PCB
Symbols (if not Components
in Library) Placed
Outside PCB
Outline

Define PCB Outline
Output for
(Board Wizard) Place Components Route PCB Re-Annotate PCB Works?
Manufacture
Define Design Rules

Production

Figure 1Overview of the PCB Design Process

The diagram above shows an overview of the PCB design process from schematic entry
through to PCB design completion.

PCB Design Training Manual 1

2 The PCB Editor Workspace

2.1 PCB Editor Panel
The various sections of the PCB editor panel are described below.

2.1.1 Browse Section
This section allows you to list, locate or edit the
following PCB object types:
• Nets
• Components
• Libraries
• Component Classes
• Net Classes
• Design Rule Violations
• Design Rules
When you select an object in the Browse section,
you can view its location in the workspace in the
MiniViewer. Each of the browse functions is
described in the following pages.

2.1.2 MiniViewer
This provides an overview of the workspace.
When you are working in the editor workspace,
the MiniViewer displays a dashed rectangle to
indicate where in the workspace the current
display window is.
When objects are selected in the browse section,
they are highlighted in the MiniViewer so that you
can locate them in the workspace.
The MiniViewer also provides the following
display control functions:
Panning Click and drag in the dashed rectangle to
pan around the workspace
Change View Window Click and drag on a
vertex of the dashed rectangle to change the view
window of the workspace
Magnifier Select the Magnifier button and then
move the cursor into the main workspace. The MiniViewer displays a magnified view of the
cursor location. You can set the magnification level by pressing the Configure button (hint –
you can also change the magnification level by pressing the SPACEBAR when the cursor is a
magnifying glass).

2 PCB Design Training Manual

2.1.3 Current Layer Section
This section indicates the current layer and its colour and allows you to change it.

2.2 Using the Panel to Browse
2.2.1 Browsing Nets

• To browse nets, select Nets in the drop down box.
All nets in the PCB are listed in the upper scroll
box.
• Click on a net name to select it and all the pads
(or nodes) that belong to that net are listed in the
lower scroll box. Also, the net is highlighted in
the MiniViewer.
• Click on the Edit button to display the Change
Net dialog box for the selected net or double-
click on the net name.
• Click on the Zoom button to display all the
connection lines for the selected net in the
workspace.
• In the Nodes section, click on an entry to select a
pad in the net.
Pad dialog box for the selected pad or double-
click on the node name.
• Click on the Jump button to zoom in the selected
pad in the workspace.


2.2.2 Browsing Components

• To browse components, select Components in
the drop down box. All components in the PCB
are listed in the upper scroll box.
• Click on a component name to select it and all
the pads that belong to that component are listed
(with their net name) in the lower scroll box.
Also, the component is highlighted in the
MiniViewer.
Component dialog box for the selected
component or double-click on the component
name.
• Click on the Jump button to zoom in on the
selected component in the workspace.
• In the Pads section, click on an entry to select a
pad in the component.
Pad dialog box for the selected component or
double-click on the pad name text.
• Click on the Jump button to zoom in on the
selected pad in the workspace.


2.2.3 Browsing Libraries

• To browse libraries, select Libraries in the drop down
box. All libraries in the current library list are listed in
the upper scroll box.
• Click on a library name to select it and all the
components that belong to that library are listed in the
lower scroll box.
• Click on the Add/Remove button to display the PCB
Libraries dialog box to add of remove libraries from the
current library list.
• Click on the Browse button or double-click on the
library name to display the Browse Libraries dialog
box.
• In the Components section, click on an entry to select a
component in the library. That component is displayed
in the MiniViewer.
• Click on the Edit button to switch to the Library Editor
to edit that component.
• Click on the Place button to place the selected
component in the workspace or double-click on the
component name.


2.2.4 Browsing Net Classes

• To browse net classes, select Net Classes in the
drop down box. All net classes in the PCB are
listed in the upper scroll box.
• Click on a net class name to select it and all nets
that belong to that net class are listed in the lower
scroll box.
• Click on the Edit button to display the Edit Net
Class dialog box for the selected net or double-
click on the net class name.
• In the Nets section, click on an entry to select a
net. The net is highlighted in the MiniViewer.
• Click on the Edit button to display the Edit Net
dialog box for the selected net or double-click on
the net name.
• Click on the Focus button to put the selected net
into focus.


2.2.5 Browsing Component Classes

• To browse component classes, select Component
Classes in the drop down box. All component
classes in the PCB are listed in the upper scroll
box.
• Click on a component class name to select it and
all nets that belong to that net class are listed in
the lower scroll box.
• Click on the Edit button to display the Edit
Component Class dialog box for the selected
component class or double-click on the
component class name.
• In the Components section, click on an entry to
select a component. The component is
highlighted in the MiniViewer.
Component dialog box for the selected
component or double-click on the component
name.
• Click on the Jump button to zoom in on that
component in the workspace.


2.2.6 Browsing Design Rule Violations

• To browse DRC Violations, select Violations in
the drop down box. All violation types in the
PCB are listed in the upper scroll box.
• Click on a violation type and all violations of that
type are listed in the lower scroll box.
• Click on the Details button or double-click on the
violation to display the Violation Details dialog
box for the selected violation.
• Click on the Highlight button to locate the
violation in the workspace.
• Click on the Jump button to zoom in on that
violation in the workspace.


2.2.7 Browsing Design Rules
To browse Design Rules, select Rules in the
drop down box. All Rule Classes are listed in
the upper scroll box.
Click on a Rule Class and all rules defined for
that class are listed in the lower scroll box.
Click on the Edit button or double-click on the
rule to display a dialog box to edit the selected
violation.
Click on the Select button to select all objects
affected by the selected rule.
Click on the Highlight button to highlight all
objects affected by the selected rule.

2.2.8 Exercises – Using the MiniViewer
1. In the Show/Hide tab of the Preferences
dialog box (shortcut keys OD) turn on the
Show Pad Nets and Show Pad Number
options.
2. Choose the Fit Board view command.
3. Use the MiniViewer Magnifier to display
the number and net information of pads.
4. Now, browse each object type and explore
the options


2.3 Preferences Dialog Box
The Preferences dialog box allows you to set up parameters relating to the PCB editor
workspace. This dialog box is displayed using the Tools » Preferences menu command.
Settings in this dialog box remain the same when you change active PCB files. The dialog box
has 6 tabs. The options in each of the tabs are described below:

2.3.1 Options Tab

Figure 2 Options Tab of the Preferences dialog box

Editing options section
Online DRC
When checked, any design rule violations are flagged as they occur. The design rules are
defined in the Design Rules dialog box (select the Design » Rules menu command).
Snap to Centre
When checked, the cursor snaps to the centre when moving a free pad or via; snaps to the
reference point of a component; snaps to the vertex when moving a track segment.
Extend Selection
Selection is cumulative with this option enabled. With it disabled all currently selected objects
are de-selected each time a new selection is made.


Remove Duplicates
With this option enabled a special pass is included when data is being prepared for output.
This pass checks for and removes duplicate primitives from the output data.
Confirm Global Edit
Displays a dialog box reporting the number of objects that will be altered by the global edit
and allows you to cancel.
Protect Locked Objects When checked, locked objects cannot be edited.

Other section
Rotation Step
When an object that can be rotated is floating on the cursor, press the spacebar to rotate it by
this amount in an anti-clockwise direction. Hold the shift key whilst pressing the spacebar to
rotate it in a clockwise direction.
Undo/Redo
This sets the undo stack size.
Cursor Type
Set the cursor to small or large 90 degree cross, or small 45 degree cross.
Autopan options section
Style
If this option is enabled, auto pan becomes activated when there is a cross hair on the cursor.
There are four Auto pan modes:
• Re-Centre - re-centres the display around the location where the cursor touched the
Window edge. It also holds the cursor position relative to its location on the board,
bringing it back to the centre of the display.
• Fixed Size Jump - pans across in steps defined by the Step Size. Hold the SHIFT key to pan
in steps defined by the Shift Step Size.
• Shift Accelerate - Pans across in steps defined by the Step Size. Hold the SHIFT key to
accelerate the panning up to the maximum step size, defined by the Shift Step Size.
• Shift Decelerate - Pans across in steps defined by the Shift Step Size. Hold the SHIFT key to
decelerate the panning down to the minimum step size, defined by the Step Size.
• Ballistic – Pans at maximum speed
• Adaptive – Pans at the rate set in the Speed field
Speed
Sets the panning speed for Auto-panning.


Interactive Routing section
Mode
This drop down box has three options as follows:
• Ignore Obstacle - If you select this option you can place tracks anywhere in the workspace.
If the Online DRC feature is enabled clearance violations are flagged immediately.
• Avoid Obstacle - If you select this option you can only place tracks where they do not
violate any design rules. This feature is particularly useful when using interactive routing
as it allows you to route hard up against existing objects, without fear of violating any
clearance rules.
• Push Obstacle - If you select this option the editor will attempt to move tracks out of the
way so that you can route the current track.
Plough Through Polygons
Marking this check box allows you to override the design rules so that the interactive routing
command can route within the area of a polygon.
Automatically Removal Loops
With this option enabled, loops that are created during manual routing are automatically
removed.
Polygon Repour
This has three options for determining whether a Polygon repours when edited:
Option Description
Never No automatic repour
Threshold Prompt of polygon has threshold primitives
Always Polygon always repours

Component Drag
This option determines how connected tracks are dealt with when moving a component. When
Connected Tracks is selected, tracks drag with the component, otherwise they do not.


2.3.2 Display Tab

Display options
Convert Special Strings
When enabled, Special strings that can be interpreted on screen are displayed. Regardless of
this setting, all Special Strings are visible when output is generated.
Highlight in Full
Completely highlights the selected object in the current selection colour. With this disabled the
selected object is outlined in the current Selection colour.
Use Net Colour For Highlight
Highlights the selected net in the net colour (assigned in the Change Net dialog box). Use with
the Highlight in Full option for better results.
Redraw Layers
Forces a screen redraw as you toggle through layers, with the current layer being redrawn last.
Single Layer Mode
Displays the current layer only. Provides a method of examining what will be output on each
layer. If the current layer is a signal layer, multi layer objects are also displayed. Use the “+”
and “-” keys to toggle through the layers; press END to redraw the screen. Shift + S also toggles
this mode.


Transparent Layers
Gives layer Colours a “transparent” nature by changing the colour of an object that overlaps an
object on another layer. Allows objects that would otherwise be hidden by an object on the
current layer to be readily identified.
Show section
The check boxes is this section perform the following when checked:
Pad Nets Displays net names on pads
Pad Numbers Displays pin numbers on pads
Via Nets Display net names on vias
Testpoints ****
Origin Marker Displays the Origin Marker
Status Info Displays information about the object under the cursor in the status
bar

Draft thresholds Section
Tracks
Tracks of the width entered in the check box (or narrower) will be displayed as a single line;
tracks of greater width will be displayed as an outline (when tracks are displayed in Draft
Mode).
Strings
The number entered in this field determines which strings are displayed as text and which are
displayed as an outline box.
Strings that are placed at or less than the value stipulated (at the current zoom level) will be
displayed as text; strings that are placed at a greater value will represented by an outline box.
Layer Drawing Order Button
The PCB editor allows you to control the order in which layers are re-drawn. Press the Draw
Order button to pop up the Layer Drawing Order dialog box. The order that the layers appear
in the list is the order that they will re-draw in. The layer at the top of the list is the layer that
will appear on top of all other layers on the screen.


2.3.3 Colours Tab
This enables you to set the display colour of each layer in the PCB.

Figure 3 Colors Tab of the Preferences dialog box

The Default Colors button sets the colors the default setting. The Classic Colors button sets the
colours to the default setting of Advanced PCB version 2.


2.3.4 Show/Hide Tab
This dialog box enables you to control which object types get displayed and how they are
displayed.

Figure 4 Show/Hide tab of the Preferences Dialog box


2.3.5 Default Primitives Tab
This enables you to set the default properties for each object type in the PCB editor . Figure 11
below shows the default setting for a track.

Figure 5 Defaults Tab

If the permanent check box is not checked, the settings in this dialog box will change when
you change the properties of an object being placed.


2.3.6 Signal Integrity Tab

Figure 6 Signal Integrity Tab

To insure the accuracy of the signal integrity analysis you need to define the appropriate
component types.
Steps:
1. Click on the Add button to display the Component Type dialog box.
2. Enter the designator prefix ( e.g. R)
in the Designator Prefix field
3. Click on the down arrow in the
Component Type field to display
drop down menu.
4. Select the appropriate component
type (e.g. Resistor)
5. Note! Components which do not
have a type assigned are assumed to be of type IC


2.3.7 Exercises – Exploring the Preferences
1. Open the document Z80 Processor Board.pcb
2. Choose the Options tab of the Preferences dialog box and try the following:
3. Check the single layer mode, click on OK and change active layers by selecting the various
layer tabs. Turn single layer mode off
4. Check Transparent Layers then zoom in and view some pads with tracks connected to
them. Turn Transparent Layers off.
5. Choose the Colors tab of the Preferences dialog box.
6. Press the Classic button and choose OK.
7. Re-display the dialog box and press the default button and choose OK
8. Experiment with changing the colours of various layers
9. Choose the Show/Hide tab of the Preferences dialog box
10. Observe the effect of pressing the All Draft, All Final and All Hidden buttons
11. Zoom in on a pad and check on and then off the Show Pad Nets and Show Pad Number
options.


2.4 Document Options Dialog Box
The Document Options dialog box allows you to set parameters relating to individual PCB
documents. This dialog box is displayed using the Design » Options menu command. The
settings in this dialog box are saved with the PCB file. The options in the tabs for this dialog
box are described below.

2.4.1 Layers Tab

Figure 7 Layers tab of the Document Options dialog box

The check boxes in this dialog box allow you to turn on or off the various PCB editor layers.


2.4.2 Options Tab
The options on this tab are described below:

Figure 8 Options Tab of the Document Options dialog box

Snap X X value for the snap grid
Snap Y Y value for the snap grid
Component X X value for the component grid
Component Y Y value for the component grid

Electrical Grid
When the electrical grid is enabled, when you are executing a command which supports the
electrical grid and you move the cursor within the Grid Range value of an object assigned to a
net, the cursor will jump to that object.
Visible Kind Sets the style of the visible grid – dots or lines
Measurement Unit Sets the coordinate system to either metric or imperial.

2.5 The PCB Coordinate System
The PCB editor has a coordinate system with the origin located in the bottom left hand corner
of the workspace. This point has the coordinates of (0,0) and is known as the Absolute Origin.
The workspace size is 100 inches by 100 inches. The reference point of the coordinate system
can be re-defined at any time using the Edit » Origin » Set menu command and this sets what is
known as the Origin. The coordinate read out in the status bar gives the coordinates relative to
the Origin. The Edit » Origin » Reset menu command sets the Origin to the Absolute Origin.


There is an Origin Marker that shows the location of the Current Origin. This is displayed by
checking the Display Origin Marker check box in the Show/Hide tab of the Preferences dialog
box.
The coordinate system units can be either metric or imperial. The View » Toggle Units menu
command or the Q shortcut key toggles the coordinate system between metric and imperial.

2.6 Grids
2.6.1 Snap Grid
The Snap Grid ensures accurate movement and placement of objects. The Snap grid causes the
coordinates of a mouse click to snap to the nearest snap grid point. The Snap grid has X and Y
values and is set on the Options tab of the Document Options dialog box. (Design » Options
menu command)

2.6.2 Visible Grid
The Visible Grid displays either as lines or dots when turned on. This is independent of the
Snap Grid. The PCB editor has two visual grids that you can set and display independently.
The Visible Grids are set and they are turned on or off in the Layers tab of the Document
Options dialog box

2.6.3 Electrical Grid
The Electrical Grid setting defines the range within which the cursor will override the snap
grid to jump to another object, such as a via, pad or track when in the interactive routing
command. When the Electrical Grid overrides the Snap Grid, an octagon displays on the
cursor. When you see that octagon, you know that the cursor is precisely located on the object
it has jumped to.
The Electrical Grid is set and turned on or off in the Options tab of the Document Options
dialog box (Design » Options menu command or OB).

2.6.4 Component Grid
The component Grid is similar to the Snap Grid except that it is only active when placing or
moving components. The Component grid has X and Y values and is set in the Options tab of
the Document Options dialog box (Design » Options menu command or OB).


2.7 Shortcut Keys for Setup Options
Pressing the O shortcut key displays a menu that provides a quick way of accessing the set up
dialog boxes. The options in this menu are described below:
Option Dialog Box displayed
Board Options Options tab of Document Options
Board Layers Layers tab of Document Options
Mechanical Layers Setup Mechanical Layers
Netlist Manager Netlist Manager
Layer Stack Manager Layer Stack Manager
Classes Object Classes
From-To Editor From-To Editor
Preferences Preferences with the last tab used as the active tab
Display Layers tab of Preferences
Colors Colors tab of Preferences
Show/Hide Show/Hide tab of Preferences
Defaults Defaults tab of Preferences
Signal Integrity Signal Integrity tab of Preferences

2.7.1 Exercises – Exploring the Document Options
1. Choose the Layers Tab of the Document Options dialog box located in the Design menu.
2. Experiment with the Used on, All On and All Off buttons and with turning on and off
individual layers
3. Choose the Options Tab of the Document Options dialog box
4. Experiment with changing the various grid settings


3 Creating a New PCB

3.1 Printed Circuit Board Wizard
When you select File » New in the PCB editor, the Select Document Type dialog box is
displayed. If you want to create an empty PCB file, choose the PCB Icon on the Blank
Document tab. If you wish to use the Printed Circuit Board Wizard, choose the Document
Wizards tab and then select Printed Circuit Board Wizard to display the Board Wizard. This
takes you through a series of steps. You can select from a range of standard PCB formats and
set up design rules for the technology you will be using on that PCB. There is also an option
for custom PCB’s.

Figure 9 Board Wizard


4 Transferring Design Information to the PCB
The Synchronizer is a tool that allows the transfer of design information between the
Schematic and the PCB documents as follows:
Schematic to PCB: Component and connectivity information from the schematic is
transferred to the PCB.
PCB to Schematic: If the designators of any PCB components are edited, or the Re-Annotate
command is executed, the schematic is automatically with the new designators
You run the Synchronizer once the schematic is finished to transfer design information to the
PCB and to place components. You also run the Synchronizer to update the PCB with any
changes that have been made to the schematic after the initial Synchronization has been
performed.

4.1 Design Synchronization
To synchronize the PCB, select the Design » Update PCB menu command in the Schematic
Editor. This displays the Update Design dialog box shown below.

Figure 10 Update Design dialog box


Choose the appropriate options for your project in the Connectivity section.
• The Assign Net to Connected Copper option updates the routing net names to match the
net names of the connected pads.
• The options in the Components section are applicable when Synchronizing a previously
placed PCB.
• The Rules section allows you to control how PCB design rules are created from Layout
Directives in the schematic
• The Synchronization process then analyses both the schematic and any PCB objects
present in the PCB document. For each difference detected between the schematic and the
existing PCB, a Macro is created. This macro tells the PCB editor what action must be
performed to update the PCB document to match the schematic.
• If you are Synchronizing a new design, macros are created for the entire schematic. If you
are updating your design, macros are created for each design change.
• If there is a condition in either the schematic or the PCB file, which prevents the
Synchronizer from generating a macro for a particular action, an error results. Errors are
listed in the Error column on the Changes tab of the Update Design dialog box. The
number of errors is shown in the Status field at the bottom of the dialog box.
• To perform the actual loading of schematic data into the PCB file, i.e. to run the macros,
click on the execute button. Macros with errors do not execute.

4.2 Resolving Synchronization Errors
The table below explains the cause of each of the possible Synchronization errors:
Error A Macro is attempting to:
Net not found Add or remove a node; remove a net; or change a net name when that
net cannot be found in the PCB document.
Component not Add or remove a node when the component designator is incorrectly
found specified in the Macro or the component cannot be found in the PCB
document; remove a component; or change a footprint, designator or
comment when the component cannot be found in the PCB document.
Node Not found Add or remove a node from a component that does not have that pin;
or remove a node that does not exist in the specified net.
Net already exists Add a net name when a net with that name already exists in the PCB
document.
Component Add a component when a component with that designator already
already exists exists in the PCB document.
New footprint not Change a component footprint when the used pins on the old footprint
matching old do not match the used pins on the new footprint. This can occur if the
footprint new component has fewer pins than the old, or if the pin numbering in
the schematic, is different to the pin numbering on the footprint.


Error A Macro is attempting to:
Footprint not Add a new component or change a component footprint when the
found in Library specified footprint could not be found in any of the libraries in the
current library list and no alternative library reference could be found
in the Cross Reference file (See 4.5.3).
Alternative Add a new component or change a component footprint when the
footprint used specified footprint could not be found in any of the libraries in the
instead (warning) current library list, but it has found an alternative in the Cross
Reference File (See 4.5.3)

4.3 Summary
Most problems with Synchronizing a design generally fall into two categories.
1. Component footprints - missing components occur when: a footprint is missing from the
component information in the schematic; you have forgotten to add the required PCB
libraries to the current library list (Design » Add/Remove Library or Add/Remove Button on
the PCB Editor panel); or the footprint in the schematic does not match any PCB library
component.
2. New footprint not matching old footprint - the cause is usually that the pin numbering on
the schematic component differs from the pin numbering on the PCB footprint.

4.4 Cross Reference File
When a Macro attempts to load or change a component footprint that cannot be located in any
of the libraries, it then uses the component Comment to look-up the Cross Reference file
(ADVPCB.XRF in Design Explorer 99 SESystem directory). The Cross Reference file lists
components by their type against any appropriate footprint(s) for that component. For example,
if the component U1 was a 74LS00, but you had forgotten to include the footprint, when the
Macro to add this component was validated it would look-up 74LS00 in the XRF file. 74LS00
has DIP14 as a footprint, which would be loaded from one of the libraries in the current library
list.


4.5 Design Transfer Using a Netlist
For most situations, the Synchronizer has superseded Netlist loading. In cases where the PCB
is being designed from a schematic drawn on another EDA vendor’s schematic editor, a netlist
can be used.
Netlist loading is a method by which connectivity and component information are transferred
to the PCB Editor via a netlist. If the netlist load is successful, the PCB file will contain all
components ready to be placed within the PCB outline.
Netlist loading is performed on a new PCB file once the schematic is complete and the netlist
generated. It is also performed whenever design changes have been made to the schematic
which then need to be propagated the PCB layout. Netlist loading is also referred to as
Forward Annotation.

4.5.1 Loading a Netlist
To load a netlist select the Design » Load Nets menu command. This displays the
Load/Forward Annotate Netlist dialog box shown below.

Figure 11 Load/Forward Annotate Netlist dialog box


• Click on the Browse button, locate and select the netlist file to be loaded.
• The netlist loading process then analyses both the netlist and any PCB design data present
in the workspace. For each difference detected between the netlist and the existing design
data, a Netlist Macro is created. This macro tells the PCB editor what action must be
performed to update the design data to match the netlist.
• If you are loading a netlist for the first time, Netlist Macros will be created for the entire
netlist. If you are forward annotating your design, Netlist Macros are created for each
design change.
• If there is an condition in either the netlist or the PCB file which prevents the netlist
loading process from generating a macro for a particular action, an error results. Errors are
listed in the Error column on the Load/Forward Annotate Netlist dialog box. The number
of errors resulting from a netlist load is shown in the Status field at the bottom of the
dialog box.
• To perform the actual loading of netlist data into the PCB file, click on the execute button.
It is unwise to execute the netlist loading while there are macro errors and hence these
should be resolved before proceeding.

4.5.2 Resolving Netlist Loading Errors
The table below explains the cause of each of the possible Netlist Loading errors:
Error A Netlist Macro is attempting to:
Net not found Add or remove a node; remove a net; or change a net name when
that net cannot be found in the PCB netlist.
Component not Add or remove a node when the component designator is incorrectly
found specified in the Macro or the component cannot be found in the
PCB netlist; remove a component; or change a footprint, designator
or comment when the component cannot be found in the PCB
netlist.
Node Not found Add or remove a node from a component that does not have that
pin; or remove a node that does not exist in the specified net.
Net already exists Add a net name when a net with that name already exists in the PCB
netlist.
Component already Add a component when a component with that designator already
exists exists in the PCB netlist.
New footprint not Change a component footprint when the used pins on the old
matching old footprint do not match the used pins on the new footprint. This can
footprint occur if the new component has fewer pins than the old, or if the pin
numbering in the netlist (which comes from the schematic
component pin numbers) is different to the pin numbering on the
PCB component.


Footprint not found Add a new component or change a component footprint when the
in Library specified footprint could not be found in any of the libraries in the
current library list and no alternative library reference could be
found in the Cross Reference file (See 4.5.3).
Alternative footprint Add a new component or change a component footprint when the
used instead specified footprint could not be found in any of the libraries in the
(warning) current library list, but it has found an alternative in the Cross
Reference File (See 4.5.3)

Summary
Most problems with loading a schematic netlist generally fall into two categories.
1. Component footprints - missing components occur when: a footprint is missing from the
component information in the netlist; you have forgotten to add the required PCB libraries
to the current library list (Design » Add/Remove Library); or the footprint in the netlist does
not match any Advanced PCB library component.
2. New footprint not matching old footprint - the cause is usually that the pin numbering on
the schematic component differs from the pin numbering on the PCB footprint.

4.5.3 Cross Reference File
When a Netlist Macro attempts to load or change a component footprint that cannot be located
in any of the libraries, it then uses the component Comment to look-up the Cross Reference
file (ADVPCB.XRF in Design Explorer 99 SESystem directory). The Cross Reference file
lists components by their type against any appropriate footprint(s) for that component. For
example, if the component U1 was a 74LS00, but you had forgotten to include the footprint,
when the Macro to add this component was validated it would look-up 74LS00 in the XRF
file. 74LS00 has DIP14 as a footprint, which would be loaded from one of the libraries in the
current library list.

4.5.4 Editing Netlist Macros
The Load/Forward Annotate Netlist dialog box provides the capability to edit the netlist
macros. If you are driving your design from the schematic via the netlist, you will not need to
use these capabilities.

4.5.5 Executing the Netlist Loading
If you have resolved all the netlist macro errors, you can execute the netlist loading by clicking
on the Execute button.
This results in all the components to be placed, being placed at the centre of the PCB outline.


5 Setting up the PCB Layers

5.1 Layer Definitions
The PCB Editor has a concept of layers to represent the various elements of a printed circuit
board. When placing objects using the PCB editor, you need to consider which layer they are
to be placed on. Objects are placed on the Current layer. The display of layers is controlled
using the Layers tab of the Document Options dialog box that is displayed by the Design »
Options menu command.

The Current Layer is set by any of the following:
• Clicking on the appropriate Layer tab
• Pressing the + or – keys on the numeric pad
• Accessing the drop-down box in the Current Layer section of the PCB Editor panel
Each of the PCB editor layers is described below:
Signal Layers
There are 32 signal layers that can be used for track placement. Anything placed on these
layers will be plotted as solid (copper) areas on the PCB. As well as tracks, other objects (e.g.
fills, text, polygons, etc.) can be placed on these layers. The signal layers are named as
follows:
Top Top signal layer
MidLayer1 to MidLayer30 Inner signal layers
Bottom Bottom signal layer
Signal layer names are user definable.
Internal Planes
Sixteen layers (named Internal Plane 1–16) are available for use as power planes. Nets can be
assigned to these layers and multi-layer pads and vias automatically connect to these planes.
Internal Plane layer names are user definable.
Silkscreen
Top and Bottom Silkscreen layers are typically used to display component outlines and
component text (designator and comment fields that are part of the component description).
Mechanical Layers
Sixteen mechanical drawing layers are provided for fabrication and assembly details such as
dimensions, alignment targets, annotation or other details. Mechanical layer items can be
automatically added to other layers when printing or plotting artwork. Mechanical Layer
names are user definable.


Solder Mask
Top and bottom masks are provided for creating the artwork used to make the solder masks.
These automatically generated layers are used to create masks for wave soldering, usually
covering everything except component pins and vias. You can control the expansions for these
masks when printing/plotting by including a Solder Mask Expansion rule. Refer to the Design
Rules section for more information on the Solder Mask Expansion rule.
Paste Masks
Top and bottom masks are provided to generate the artwork which is used to manufacture
stencils to deposit solder paste onto surface mount pads on PCB’s with surface mount devices
(SMDs). Refer to the Design Rules section for further information.
Drill Drawing
Coded plots of board hole locations typically used to create a drilling drawing that shows a
unique symbol for each hole size at each hole location. Individual layer pair plots are provided
when blind/buried vias are specified. Three symbol styles are available: coded symbol,
alphabetical codes (A, B, C etc.) or the assigned size.
Drill Guide
Plots of all holes in the layout - sometimes called pad masters. Individual layer pair plots are
provided when blind/buried vias are specified. These plots include all pads and vias with holes
greater than zero (0) size.
Keep Out
This layer is used to define the regions where components and routes can validly be placed.
For example, the board boundary can be defined by placing a perimeter of tracks and arcs,
defining the region within which all components and tracks must be placed. “No-go” areas for
components and tracks can be created inside this boundary by blocking off regions with tracks,
arcs and fills. Keep outs apply to all copper layers. The basic rule is; components can not be
placed over an object on the Keep Out layer and routes can not cross an object on the Keep
Out layer.
Multi Layer
Objects placed on this layer will appear on all copper layers. This is typically used for through
hole pads and vias, but other objects can be placed on this layer


Display Layers
The layers described below cannot have objects placed on them but they are turned on or off in
the Design-Options dialog box.
DRC Errors
This option controls the display of the Design Rule Check (DRC) error marker.
Visible Grids
Controls the display of the two visible grids.
Pad and Via Holes
Controls the display of pad and via holes. To be able to distinguish pads from vias in draft
mode, pad holes are outlined in the current Pad Holes colour (set in the Colours Tab of the
Preferences dialog box).
Connect
This option controls the display of the connection lines. The PCB editor displays
connection lines wherever it locates part of a net that is un-routed.


5.2 Layer Stack Manager
The Layer Stack Manager provides an easy to use, graphical method of defining, naming and
editing layers. It is displayed by selecting the Design » Layer Stack Manager menu command
(DK).

Figure 12 Layer Stack Manager

The Layer Stack Manager allows you visually see the “stack up” of your PCB, i.e. the
relationship between copper, substrate and prepreg.
Adding a Signal Layer
To add a layer to your PCB, click on the name text of an existing layer displayed in the Layer
Stack Manager and the click on the Add Layer button or right click and choose Add Signal
Layer from the right click menu. This procedure adds a new layer with a default name
allocated to it. Double-clicking on the name text for that layer enables you to edit the name or
the copper thickness of that layer.
Adding An Internal Plane Layer
To add an Internal Plane layer to your PCB, click on the name text of an existing layer
adjacent to where you want the plane inserted then click on the Add Plane button or right click
and choose Add Internal Plane Layer from the right click menu. This procedure adds a new
internal plane layer with a default name allocated to it. Double-click on the name text for that
internal plane layer to edit the name, the copper thickness or net name for that layer.


Insulation Layers
As additional layers are added to the PCB, insulation layers are automatically added. The
insulation layer can either be Core or Prepreg and this is determined by the “Stack Up” style
setting. Double-clicking on the name text sets the properties of the insulation layers. These
properties are material, thickness and Dielectric constant. The Signal Integrity software uses
these properties.
Deleting a Layer
To delete a layer, click on the name text of an existing layer and then click on the Delete
button or right click and choose delete from the right click menu.
Editing the “Stack Up” Order
To change the order in which layers are defined in your PCB, click on the name of the layer
and click on the Move Up or Move Down buttons or Right Click and choose Move Up or
Move Down from the right click menu.
Editing the “Stack up” Style
The “Stack Up” style defines the order in which the PCB substrate, copper and prepreg
insulation layers are fabricated as well as the finish on the PCB. The Style is set in the top left
hand corner of the Layer Stack Manager. The “Stack up” is specified in the drop down box.
The choices are:
• Layer Pairs
• Internal Layer Pairs
• Build Up
The board finish is defined by selecting the buttons next to the Top and Bottom Dielectric
check boxes. Click on these to set the material, thickness and dielectric constant for the finish.
Drill Pairs
The term Drill Pairs refers to the two layers that a drilling operation starts from and finishes at.
By default Drill Pairs are defined as Top and Bottom Layers. If blind or buried vias are to be
used on your PCB, Layer Pairs must be defined for these. Pressing the Drill Pairs button
performs this.


5.3 Defining Mechanical Layers
Before a Mechanical Layer can be used it must be enabled in the Setup Mechanical Layers
dialog box that is displayed by selecting the Mechanical Layers command in the Design menu.
Marking an Enabled check box enables a Mechanical Layer. Once enabled, the layer name is
displayed and can be edited.

Figure 13 Setup Mechanical Layers Dialog Box

The visible check box allows you to control the display of its mechanical.
When checked, the Display In Single Layer Mode check box causes its layer to be displayed
when Single Layer Mode is invoked (Shift S).


5.4 Internal Power Planes
General Notes
The PCB Editor allows for up to sixteen power planes.
A power plane is defined by assigning a net to an internal plane layer.
The PCB editor automatically connects pins that belong to the power plane net and isolates all
other pins from the plane.
Internal power planes are output as photographic negatives (compared to other layers which
are output as positives).

5.4.1 Defining an Internal Power Plane
An internal power plane is added, named and assigned to a net using the Layer Stack Manager.
When a net has been assigned to an internal plane layer, pins in that net automatically connect
to that plane layer using thermal relief connections. The style of these is defined in the Power
Plane Connect Style rule class in the Manufacturing tab of the Design Rules dialog box. Nets,
which are not connected to the plane, are isolated from it by a clearance which is defined in the
Power Plane Clearance rule class in the Manufacturing tab of the Design Rules dialog box

5.4.2 Defining a Split Power Plane
Internal power planes have the capability to have multiple nets on the same Internal plane layer
by using the Split Planes object. The additional nets must be within enclosed areas on the
internal plane as shown in Figure 14.

Internal Plane

Split Plane

Figure 14 Split Plane Example


To define a Split Plane, select the Place » Split Plane menu command. This displays the Split
Plane dialog box shown in Figure 15where you enter the track width, internal plane layer and
net for the split plane. The track width you key in is actually the width of the isolation region
between the internal plane net and split plane net.

Figure 15Split Plane dialog box

Tip: To help ensure that you enclose all the required pins in the split plane; you can change the
colour of the split plane net. Use the Browse Net function on the PCB Editor panel and then
use the Select » Physical Net menu command to display the pins with their net colour.

5.4.3 Moving and Editing Split Plane Vertices
You can move the split plane by clicking and holding on the split plane track and moving it to
a new position. You can move and insert vertices on the split plane using the Edit » Move »
Split Plane Vertices menu command.

5.4.4 Deleting a Split Plane
To delete a split plane, select the Edit » Delete command and then click on the split plane to be
deleted.


5.4.5 Exercises – Setting up the PCB Layers
Assigning an Internal Plane
1. Open the document Z80 Processor Board.pcb
2. Using the Design » Layer Stack Manager menu command, assign the net GND to Internal
Plane 1. Observe the connection lines for the GND net when you do this.
3. Turn all layers off except Internal Plane 1 and zoom in on pins that belong to the GND net.
4. Placing a Spilt Plane for the +12V Net
5. So that the +12V pads can be seen, use the Net browser in the PCB editor panel to edit the
net +12V and change its colour to a unique colour.
6. In the Options tab of the Preferences dialog box, turn on the Use Net Colour For Highlight
option and then select the Edit » Select » Physical Connection menu command -You
shouldn’t see the +12V pads shown in a different colour to the rest of the pads.
7. Place a +12V split plane on Internal Plane 1 (make sure to enclose some +12Vpads)
8. Now move the split plane so that it encloses a GND pad. Observe that the GND enclosed
GND pad becomes isolated from the +12V copper.
9. Use Edit » Delete to delete the split plane. Note the effect on the +12V pads.


6 Setting Up Design Rules
General Notes
Traditionally, the term Design Rules referred to PCB editor functions that ensured that your
design complied with predetermined manufacturing requirements (e.g. minimum clearances in
copper). In addition, they were applied globally to the PCB.
In recent times, Protel has expanded the concept of Design Rules. They now apply to every
aspect of the PCB design and optionally to specific objects as well as globally.
This section describes how Design Rules are defined. The following section describes how to
check for design rule violations.

6.1 Adding Design Rules
Design rules are defined in the Design Rules dialog box that is displayed by selecting the
Design » Rules menu command.

Figure 16 Design Rules dialog box

To set up a design rule:
• Click on the tab to select the general category for the rule
• In the Rule Classes list, single click on a specific rule to display a definition of the rule
• Double-click on a specific rule to display the dialog box where you can set the Rule Scope
and Rule Properties for that rule.
To see the objects affected by a rule, click on the Select Affected Objects button at the bottom
of the Design Rules dialog box. This selects the affected objects.


To effectively apply the Design Rules, the concepts of Object Set, Scope, Rule Type and
Precedence need to be understood. These are described in the following sub-sections.

6.2 Object Set
This refers to the object or group of objects a rule applies to. The Object Set can be a single
object or a group of objects determined by the Rule Scope.

6.3 Rule Type
There are two types of Design Rules as follows:
Unary Design Rules Binary Design Rules
These apply to one object, or each object These apply between two objects, or between
in a set of objects any object in one set to any object in the second
set.
e.g. Solder Mask Expansion
e.g. Clearances, which apply between any
Unary rules have one section on the left
hand side of the Edit Rule tab of their copper object in the first set and any copper
object in the second set, as identified by the two
dialog box.
rule scopes.
Binary rules have two sections on the left hand
side of the Edit Rule tab of their dialog box
designated A and B.

6.4 Scope
This allows you to determine how the rule is applied. Some rules do not support all Scopes.
The options for scope are:
Scope Description
Region A rectangle within the board area defined by diagonal coordinates
Pad A specific pad on the board (e.g. U2-4)
Pad Specification Pads defined by their properties (e.g. size, hole size, net)
Pad Class A user defined group of Pads
Via Specification Vias defined by their properties (e.g. diameter, hole size)
From-To A specific connection from one pad to another (Defined in Design »
From-To Editor menu)

From-To Class A user defined group of From-To’s (Defined in Design » Classes menu)
Footprint A specific library component designated by footprint
Footprint Pad A specific pad of a footprint
Net A specific net
Net Class A user defined group of nets (Defined in Design » Classes menu)


Component A specific component
Component Class A user defined group of components (Defined in Design » Classes
menu)
Object Kind A type of primitive object
Layer A routing layer (Top, mid 1-30 or bottom)
Whole Board Applies to the complete PCB design

Multiple Scopes can be applied to the same Object Set by clicking on the And tab for the
Object Set

6.5 Precedence
Through the use of different scopes it is possible to have conflicting rules applied to the same
object. There is an order of precedence of scope that applies to resolve these conflicts. The
order of precedence of scope is listed below:
Region (highest priority)
Pad
Footprint-pad
Via Specification
Pad specification
Pad class
From-To
From-To Class
Net
Net Class
Component
Component Class
Footprint
Object Kind
Layer
Whole Board (lowest priority)


6.6 Where Rules Apply
6.6.1 Routing Rules

Rule Class Place Auto On-Line Batch Output Other
Track Route DRC DRC Generation
Clearance Y Y Y Y Place
Constraint Polygon
Routing Corners Y
Routing Layers Y
Routing Priority Y
Routing Topology Y
Routing Via Style Y
SMD Neckdown Y Y
Constraint
SMD To Corner Y Y
Constraint
SMD To Plane Y Y
Constraint
Width Constraint Y Y Y Y

6.6.2 Manufacturing Rules

Rule Class Auto On-Line Batch DRC Output Other
Route DRC Generation
Acute Angle Y Y
Constraint
Hole Size Constraint Y Y
Layer Pairs Y Y Y Place Track
Minimum Annular Y Y
Ring
Paste Mask Exp Y
Polygon Connect Place Polygon
Style
Power Plane Y
Clearance
Power Plane Connect Y Internal Planes
Style
Solder Mask Exp Y
Testpoint Style Y Y Y Y Find Testpoint
Testpoint Usage Y Y Y Y Find TestPoint

6.6.3 High Speed Rules

Rule Class Auto On-Line Batch Output Other
Route DRC DRC Generation
Daisy Chain Stub Y
Length
Length Constraint Y Y
Matched Length Y Y Equalise Net
Nets Lengths command
Maximum Via Y Y
Count Constraint
Parallel Segment Y Y
Constraint
Vias Under SMD Y Y
constraint

6.6.4 Placement Rules

Component Y Y Auto Place
Clearance
Constraint
Component Auto Place
Orientation
Nets To Ignore Auto Place
Permitted Layers Auto Place
Room Definition Y Y

6.6.5 Signal Integrity Rules
All Signal Integrity rule apply only to Signal Integrity Analysis

6.6.6 Other Design Rules

Short Circuit Y Y
Constraint
Un-Connected pin Y
Constraint
Un-routed Net Y Y
Constraint


6.7 Additional Information on Rules
SMD to Corner Constraint
This rule specifies the minimum distance that should be allowed from the centre of a surface
mount pad to the first vertex of a track routed to that pad.
Width Constraint
This rule allows you to apply and maximum and minimum track width to tracks determined by
the scope selected. When this rule is applied, it overrides the default track width.
Matched Length Nets Rule
This rule can be applied to Net Classes and From-To Classes. When applied, it determines the
longest Net or From-To in the class and sets any that fall outside the tolerance as violations.
The violations can be automatically corrected using the Tools » Equalize Net Lengths
command. This command attempts to lengthen nets in violation by inserting “accordion”
sections to the track provided it does not violate Clearance Constraint design rules.

Figure 17 Matched Lengths Rule Dialog Box

Short Circuit Constraint
This rule allows you to overrule the short circuits by specifying Nets or Net Classes that can be
connected together. This rule is provided to allow for situations where a mixed signal PCB has
multiple ground signals that must be connected together at one point on the PCB.


6.8 Object Classes
6.8.1 Defining Classes
Classes are provided to enable various commands to operate on sub-sets of object types. eg, a
group of components.
Commands will operate on a class if a design rule for that class has been defined.
Classes can be applied to:
• Nets
• Components
• Pads
• From to’s
To assign an object type to a class, choose the Design » Classes menu command. This displays
the Object Classes dialog box shown in Figure 18 below.
Click on the tab for the object type you want to assign and press the Add button. This displays
a dialog box such as the Edit Component Class dialog box shown below. You enter a new
name for the class to be defined in the Class Name field. The Non-Members scroll box lists all
the objects (of that object type) in the PCB file. Objects are assigned to the class by clicking on
the object name and then pressing the > button which transfers the object name to the
Members scroll box. Objects can be removed from the class by click on the name in the
Members scroll box and pressing the < button.

Figure 18 Assigning Object Classes


Once classes have been defined, objects can be added or removed by clicking on the class
name and pressing the Edit button on the Object Classes dialog box and Classes can be deleted
press the Delete button.
Any object of a particular type can belong to more than one class.
Each Object Class tab provides the option to add or remove objects from a class based on
selection.
Also, objects can be selected by Class by clicking on the Select push button.

6.8.2 Component Class Generator
The Edit Component Class dialog box has the Class Generator button. When clicked, the
Component Class Generator dialog box displays.
This allows you to define a component class containing components based properties selected
properties.


6.9 From To’s
The PCB editor provides the capability of having commands operate on a particular pin-to-pin
connection in a net, in a different manner to the rest of the net. A specific pin-to-pin
connection is defined as a From-To. Commands will operate on a From-To if a design rule for
that From-To has been defined.
A From-To is defined using the From-To Editor that is invoked using the Design » From-To
Editor menucommand. This displays the From-To Editor shown in Figure 19.

Figure 19 From-To Editor

From the net you want to assign From-To’s in, you click on that net name in the drop down
box in the net section, this displays the pads assigned to that net in the graphical window. The
display colour of the pads shows their electrical type.
To assign a from-to, click on the ‘to pin’ in the graphical window, then click on the ‘from pin’
and then right click and choose Add From-To from the menu that pops up. This adds a new
From-To to the From-To’s list and displays the From-To in the graphical window.
When you move the cursor over a pad in the graphical window, the designator and pin number
of the pad is displayed immediately below the graphical window. Double-click on a pad to edit
its properties.
To remove a From-To, click on the From-To name or the From-To in the graphical window,
then right click and choose Remove From-To from the menu that pops up.
The Auto Generate section allows you to assign From-To’s for a complete net to a specific
topology.


7 Component Placement Tools
General Notes
Once Components are placed in the file after running the Synchronizer (Design » Update PCB
in the Schematic editor), you can make use of all the following placement tools to achieve a
final placement:
• Move Component
• Auto Placement
• Interactive Placement
The quality of the component placement may determine whether or not your design can be
routed.

7.1 Placing Components With Predetermined Locations
Almost every PCB will have some components that must be placed in a specific location.
These typically include connectors, switches and indicating lights.
If you can visually locate such components, click and hold on the to move them.
Otherwise, select the menu command Edit » Move » Component and then give a mouse click
where there are no objects. This displays a dialog box in which you could enter the Designator
of the component to be placed. If you press ENTER, a list of all Designators is displayed.
From this list, you can select the component to be placed and that component will appear on
the cursor ready to be placed. Press the TAB key to display the Component dialog box and in
the Properties tab, check the Locked check box. This will lock the component so that it will
not be moved by other placement commands.
Repeat this for all components with pre-determined locations.

7.2 Moving Components
Click and hold on a component to move it. While you are moving the component, the
Connection Lines directly connected to it will drag with it while all other Connect Lines are
not displayed. As you move the component Connect Lines are dynamically optimised such that
every Connect Line is following the shortest path to any other object with the same net name.
You will also notice that as you click and hold on a component, a thicker line with a dot at
either end displays. This “placement quality vector” indicates the distance from the optimum
placement position for that component, based on connect line length. This will help you decide
on the best location for each component as you are refining the placement.
Also, while you are moving a component, pressing the N key will toggle the display of
connections.
Pressing the L Key while moving a component toggles the component between the top and the
bottom of the PCB.

7.3 Component Unions
The Union feature allows you to group components together so that they can be moved as a
group as if they were a single component. Multiple Unions can be defined.

To create a Union of components, select the components then choose the Create Union
command on the Component Placement toolbar.
To remove a component from a Union or to remove the Union, choose the Break Union
command on the Component Placement toolbar. This displays a dialog box that lists all
components in the Union. From here, select the component(s) to be removed from the Union.
Selecting all components removes the union.

7.4 Rooms
A room is a rectangular object that defines an area where components can either be kept within
or kept out of. These rectangular objects are called Room Definitions. They are placed using
the Place » Room menu command or from the Placement toolbar. Once a room definition
object is placed, you define the components associated with it and whether they are to be kept
in or kept out in the Placement tab of Design Rules.
If a component is moved such that it is in violation of the Room Definition rule, it is displaced
with a DRC marker.
There is also an Arrange Within Room command that places components within the room they
have been assigned to.

7.5 Component Placement Grids
When Placing or Moving components, they “snap” to the Component Placement grid. This
grid has an X and a Y value and they are set in the Option tab of Document Options.

7.6 Density Map
The Density Map command is provided to allow you to evaluate the quality of your component
placement. It generates a graphical display of the connection density of the PCB layout. It is
analogous to a thermal contour map. The “hot” areas, which display in red, indicate areas that
are too dense to successfully route. Look at any red areas and try to create more routing space.
To display the Density Map, select the Tools » Density Map command. When you are finished
with the density map, select the View » Refresh command or the End shortcut key to display
the PCB editor workspace.


7.7 Interactive Placement Commands
There are a number of “semi-automated” tools that allow you to edit the placement of your
PCB design. They are accessed via the Tools » Interactive Placement menu and the Component
Placement toolbar. These are described in the following sub-sections.

7.7.1 Alignment Commands
Use these to ‘fine tune’ your component placement. The Alignment commands operate on any
selected components.

7.7.2 Arrange Commands
These automatically move components as follows:
Arrange Within Room Components assigned to the nominated room
are placed within that room
Arrange Within Rectangle Selected components are placed with an area
Arrange Outside Board All unlocked components are moved outside the
board area

7.7.3 Move To Grid
All Unlocked components are moved to the closest Component Placement Grid point.

7.8 Auto Placement
The Automatic Placement attempts to optimally place all components in the PCB file, which
are not locked. It uses the largest enclosed shape on the Keep Out layer to determine the space
available for placement and will not place components in any enclosed shapes on the Keep Out
layer within the board outline. The PCB editor provides two options for Auto Placement, both
using a different method of calculating and optimising component positions suiting to different
board densities. These options are:
• Cluster Placer: groups components into clusters based on their connectivity, and then
places these clusters geometrically. The algorithms in this auto placer are more suited to
designs with a lower component count (less than 100).
• Statistical Placer: uses a statistical algorithm to place the components in an attempt to
minimise the connection lengths. As it uses a statistical algorithm it is best suited to
designs with more than 100 components.


7.8.1 Cluster Placer
To run the Cluster Placer, select the menu command Tools » Auto Place and this displays the
Auto Place dialog box shown below. Click on the Cluster Placer radio button. The Cluster
placer adheres to the Placement rules defined in the Design Rules.

Figure 20 Autoplace dialog box

7.8.2 Statistical Placer
To run the Statistical Placer, select the menu command Tools » Auto Placement and this
displays the Auto Place dialog box shown above. Click on the Statistical Placer radio button
The parameters you can set Statistical Placer are described below:
• Group Components that are “tightly” connected are grouped together and effectively
treated as one component for Auto placement.
• Rotate Components Allows components to be rotated
• Grid This is the grid each component reference point will be placed on.
Power Nets and Ground Nets Fields
This section performs the following functions:
As a power net is typically connected to most components, little is achieved by attempting to
optimise it. Any nets entered in this these fields will not be considered by the Auto Place
process. Using this option will speed up the Auto Placement.
Any components connected to both these nets will be considered to be de-coupling capacitors
and will be grouped with large components (greater than 14 pins).
Note: Before running the Statistical Auto Placer, you should set the origin to the Absolute
Origin (Edit » Origin » Reset).


Once the parameters have been set, click on OK. This launches the Auto Placer, which runs in
a separate editor window.
You can stop the Auto Placer at any time by closing the Auto Placer window. You are then
prompted as to whether you want to update the PCB file with the current placement.

7.8.3 Shove
This command allows you to place a component on a PCB so that it slightly overlaps other
components on the board, and then automatically shoves the overlapping components to allow
the new component to fit.
The Shove commands are located in the Tools » Auto Placement menu.
To do this, select Shove from the Tools » Auto Placement menu. The cursor will change to a
crosshair. Position the cursor over the component that is to be positioned on top of other
components and left-click or press ENTER. All the components that surround the selected
component and are in contact with it will be moved aside to make room for the component,
clearances permitting.
If a shoved component hits the edge of the Keep Out perimeter, there will be a "bounce back"
effect and that component will back away from the edge and shove the other components until
there is no overlap. To avoid shoving a particular component, enable its Locked attribute.
To control the "ripple" effect that shoving can produce, you can limit the number of
subsequent component shoves (those produced by the initial shoved components) set the
Shove Depth. A setting of "1" means that only the components which directly violate the
"target" component will move until they are clear of the target. Setting the depth to "2" means
that the process is repeated, allowing the newly shoved components to shove any components
that they now overlap. Setting the depth to higher numbers allows more iterations of the
process. To avoid unpredictable results on complex and dense designs, it is advisable to set the
shove depth to a low number (the default is 1).


7.9 Re-Annotation
The PCB Editor provides the Re-Annotation command to re-number component designators,
such that they are numbered in some kind of order. To do this, choose the Tools » Re-Annotate
menu command. This displays the Positional Re-Annotate dialog box shown below. You
select the Method by which you want the re-annotation to be performed and then click OK.
Alternatively, you edit individual component designators by double-clicking on the
component.

Figure 36 Positional Re-Annotate dialog box
You can update the Schematic with the designator changes using the Synchronizer. To do this,
select Design » Update Schematic.


8 Routing

8.1 Interactive Routing
The Interactive Route command has some very powerful features that are available when
placing tracks. These are described below.

8.1.1 Managing Connectivity
Once components are placed into a PCB file, Connection Lines display to indicate un-
connected nets. Whenever there is an operation on a copper layer which effects connectivity,
the PCB editor analyses the PCB to determine if any connections have changed. If any
connections have been made by tracks, connection lines are no longer displayed. Also, if a
shorter path for any connection is created by a new connection, a shorter connection line is
displayed.

8.1.2 Track Width
When using the Interactive Routing command, the setting for Preferred Width in the Width
Constraint design rules determines the track width.

8.1.3 Interactive Routing Mode
Interactive Routing Mode is set in the Options tab in the Preferences dialog. If it is set to
‘Avoid Obstacle’, you cannot place a track in violation of the design rules. If it is set to ‘Push
Obstacle’, tracks in the path of the track being placed are automatically pushed aside to allow
it to be routed.

8.1.4 Look Ahead Routing
The PCB editor incorporates the “look-ahead” feature that operates as you place tracks. The
track segment that is connected to the cursor is a look-ahead segment (displays in outline/draft
mode). The segment between this look-ahead segment and the last-placed segment is the
current track that you are placing (displays in final mode).
Use the look-ahead segment to work out where you intend to place the next segment and to
determine where you wish to terminate the current segment. When you click to place the
current segment, its end point will be positioned exactly where you need to commence the next
segment. This feature allows you to quickly and accurately place tracks around existing objects
and plan where the next track segment can be placed.
As you use the look-ahead segment to guide your routing, you will notice that the track end
does not always remain attached to the cursor. It “avoids” electrical objects that belong to
another net. This feature prevents you from violating any clearance constraints.

8.1.5 Interactive Routing Properties
When using Interactive Routing, track width is determined by the Width Constraint design
rules. Pressing the tab key while routing displays the Interactive Routing dialog box, where
you can set width and via properties.


8.1.6 Loop Removal
The Loop Removal Function is activated automatically when the Interactive Routing command
is in use. This feature helps you to edit a track once you have placed it. For example, you
realise that a track you have placed occupies a routing channel that you need for another track.
Editing a Track Using the Loop Removal Feature
Select the Place » Interactive Routing command.
Position the cursor on the section of track you wish to edit.
Click to initiate the starting point of the new track section.
Place the new track.
Click on the existing track section to finish placing the new track section.
Notice that the old track disappeared when you clicked to place the finish point of the new
track!
Note: The loop removal function only works if both the starting point and the finishing point
of the new track lay within the original track section (i.e. no pads can be within the section
being edited).
If you do not want this function to operate while you are placing tracks:
• Press the OP on your keyboard to display the Preferences Dialog box
• Unmark the Loop Removal box in the Options tab
Electrical Grid
When in the interactive routing command, an octagonal graphic displays on the cursor
whenever the Electrical Grid snaps the cursor to an object assigned to a net.


8.2 Automatic Routing
General Notes
• The automatic router is a Shape Based Router that uses Neural Net techniques to assign
routing parameters to each connection.
• You can learn more about Advanced Route by reading the ‘Autorouting a Printed Circuit
Board’ section in Help (you will find it in Help Contents)
• Where appropriate, design rules are adhered to by the autorouter.

8.2.1 Automatic Routing Tips

• The board must include a closed boundary on the keep out layer.
• You can protect pre-routed connections, fan-outs and entire nets by enabling the Protect
Pre-routes option in the Autorouter Setup dialog. This option also protects fan outs and
partially routed connections.
• Objects with a net name that are not locked may be moved/ripped up during routing.
• Objects placed on the keep out layer create blocks for the router on all layers.
• Signal layer objects with no net name create blocks for the router on that signal layer.
• The router does not consider objects on the mechanical layer.

8.2.2 Setting Up the Automatic Router

• The Autorouter requires minimal set up. Select Auto Route » Setup to display the
Autorouter Setup dialog box shown below.

Figure 21 Autorouter Setup dialog box


You simply click on the check boxes next to the Route Passes you would like performed. For
an unrouted PCB, you would most likely check all of them.

8.2.3 Autorouter Options
Once the Autorouter has been set up, you can choose any of the following options in the Auto
Route menu:

All Routes the complete PCB
Net Routes a complete net. You are prompted to select the net
Connection Routes a connection within a net as defined by a connection line. You
are prompted to select the connection
Component Routes all connections to a component. You are prompted to select the
component
Area Routes all connections within an area. You are prompted to define the
area.

At any time while the PCB is being routed you can temporarily stop it using the Auto Route »
Pause menu command and re-start it using Auto Route » Start.

The routing can be terminated using the Auto Route » Stop command. Any connections made
by the autorouter are kept.
Any or all of the connections made by the autorouter can be removed using the un-route
commands in the Tools menu.


9 Polygons
General Notes
• A polygon is an area of copper on a signal layer, usually connected to a net, that is
“poured” over existing objects, such as tracks and pads.
• They can be solid or hatched.
• They maintain a clearance, set in the design rules, away from other copper objects.
• They are made up of tracks and arcs but is recognised as a single object.
• They can be any enclosed shape comprising lines and arcs.
• They can be placed on other layers but do not pour around other objects when not placed
on signal layers.

9.1 Placing a Polygon

Place a polygon using the Place » Polygon Plane menu command or this toolbar button.
This displays the Place Polygon Plane dialog box in which you set up the parameters for the
polygon.

Figure 22 Polygon Plane dialog box


The parameters for Place Polygon are listed below:
Net Options
Connect to Net Select the net to connect the polygon to
Pour Over Same Net Existing tracks within the polygon which are part of the net being
connected to will be covered by the polygon.
Remove Dead Copper Removes any part of the polygon that cannot connect to the plane
net

Plane Settings
Grid Size Spacing between tracks that make up the polygon
Track Width Width of tracks that make up the polygon
If Track Width is equal to the Grid Size, the polygon ends up as
solid copper.
If Grid Size is greater than Track Width, the polygon ends up as
hatched.
Layer Select the signal layer that the polygon is to be place on.
Lock Primitives If unchecked, individual objects (i.e. tracks or arcs) that make up
the plane can be deleted.

Hatch Style
90-Degree Hatch Polygon is hatched with horizontal and vertical tracks
45-Degree Hatch Polygon is hatched with tracks at 45 degrees and 135 degrees
Vertical Hatch Polygon consists of only vertical tracks
Horizontal Hatch Polygon consists of only horizontal tracks
No Hatching Only outlines are poured

Surround Pads With
Octagons Places a track to form an octagon around pads
Arc Places an arc around pads

Minimum Primitive Size - Tracks or arcs below this setting are not placed

9.2 Editing a Polygon
Once a polygon has been placed, either double-clicking on the polygon or selecting the Edit »
Change menu command and clicking on the polygon can change any of the parameters, which
you set in the Place Polygon dialog box. This displays the Place Polygon dialog box where you
can change any of the parameters and then click OK. You are then prompted to re-pour the
polygon.


9.3 Moving a Polygon
Move a polygon as you would any other object. Click and hold and move it to the next
location. When you release the mouse button, you are prompted to re-pour the polygon.

9.4 Editing Polygon Vertices
To move or insert vertices on a polygon, select the Edit » Move » Polygon Vertices command
and click on the polygon to be moved. This polygon will display handles at each vertex and a
small cross the centre point of each line segment of its border. To move a vertex, click and
drag on the handle for that vertex. To insert a vertex, click and hold on the cross in the line
segment and drag it to where the vertex is required.

9.5 Deleting a Polygon
To delete a polygon, select the Edit » Delete command and then click on the polygon to be
deleted.

9.6 Exercises – Working with Polygons
1. Open the file Z80 Processor Board.pcb
2. Place a Polygon Plane covering 3 or four IC’s using the parameters in the Polygon Plane
dialog box shown in Figure 22.
3. Double-click on the polygon to edit it and change the grid sizes to 25mil and Hatching
style to 45-Degree Hatch and then re-pour the polygon.
4. Click and hold on the polygon and move it by 2 snap grid points.
5. Use the Edit » Move » Polygon Vertices menu command to change the shape of the
polygon.
6. Use Edit » Delete to delete the polygon.


10 Design Rule Checking
• The Design Rules Checking (DRC) functions are provided to check that your design
conforms to the design rules.
• There are both On-line and Batch DRC functions.
• A design should only be submitted for manufacturing when all DRC violations have been
resolved.
• DRC violations can be located using the Violations browser in the Browse section of the
PCB Editor Panel

10.1 On-Line DRC
If the On-Line DRC option is turned on, any DRC violations cuase are marked as you create
them. Checking the On-Line DRC check box in the Options Tab of the Preferences dialog box
turns on the On-Line DRC.
You can configure which Design Rules are checked by the On-Line DRC from the On-Line
Tab of the Design Rule Checking dialog box shown in Figure 23. This dialog box is displayed
by selecting the Tools » Design Rule Check menu command.

Figure 23 On-Line Tab of the Design Rule Checking dialog box


The interactive routing command has an addition On-Line DRC function as detailed in the
table below:
Interactive Routing Mode parameter in the On-Line DRC action when
Options tab of the Preferences dialog box rules are violated
Avoid Obstacle Prevents track being placed
Ignore Obstacle Places DRC marker
Push Obstacle Moves obstacle

10.2 Design Rules Check Report
This is often referred to as the Batch DRC. This performs design rules checks based on the
options selected. Selecting the Tools » Design Rule Check menu command runs the DRC. This
displays the Design Rule Checking dialog box shown in Figure 24. This will run a DRC check
on the PCB and mark any violations found.

Figure 24 Report Tab of the Design Rules Checking Dialog box

The Rules sections of this dialog box enable you to select which design rules the DRC will
check violations for.
Note the ‘All On’ and ‘All Off’ buttons in these sections. They either check or un-check all
options in the section.

10.3 Locating Design Rule Violations
The following are provided to locate DRC violations:
Violations browser in the Browse section of the PCB Editor Panel


Jump to Error Marker Select this command using Edit » Jump » Error Marker. When
invoked, the PCB editor locates the next DRC violation and zooms in on it and displays in
centre screen. Each time this command is selected, the next Error marker is displayed. You can
also use the Jump command to jump to components, nets, pads, strings or coordinates.
Cross Probing To use Cross Probing, switch to the DRC report file in the Text editor. Select
the text relating to the object that you would like to locate in the PCB editor. This can be any
of the following:
• Designator
• Designator-Pin
• Coordinate
• String

Then select the Cross Probe toolbar button in the text editor toolbar. Switch to the PCB
editor and the selected object will be displayed centre screen.

10.4 Exercise
1. Open the PCB in the Z80 Microprocessor database.
2. Define a Clearance Constraint design rule to ensure that the RAWBAUD net maintains a
clearance of 200 mils from the net 19200.
3. Route these nets using the interactive routing command with Push Obstacle on.
4. Test that the rule prevents you from creating a violation


11 Printing
Printing from your PCB document is performed using Protel’s Print/Preview utility. This
allows you to control the complete printing process from definition of layers to print,
previewing and printing.

11.1 Running Print/Preview
Print/Preview is invoked by clicking on the Printer icon on the Main toolbar or from the
Print/Preview command in the File menu. This launches the Print/Preview server that creates a
new PowerPrint Configuration document (.PPC) as shown below.

In the display window of this document, a print preview of your PCB is displayed. In the
Browse PCBPrint tab of Design Manager a list of Printouts in this document are displayed.
Clicking on the + next to the Printout icon expands out the list of layers that comprise that
printout.
To print to a printer, there are the following options:
Menu command Description
Print All Prints all Printouts
Print Job Prints all Printouts as a single print job
Print Page Prints the currently displayed preview
Print Current Prints the current Printout

Also, clicking on the Printer icon on the Main toolbar performs Print All.
The Tools menu contains the following commands for creating pre-defined Printouts:
• Create Final
• Create Composite
• Create Power Plane-Set
• Create Mask Set
• Create Drill Drawings
• Create Assembly Drawings
• Create Composite Drill Guide
• Customising a Printout
To customise a Printout, right click on the Printout icon and choose Properties. This displays
the Printout Properties dialog box shown.

To add a new layer to a Printout, right click on the Printout icon and choose Insert Print Layer.
You then need to set the properties of the new layer just added by right clicking on that layer’s
icon and choose Properties. This displays the Layer Properties dialog box shown over.


In this dialog box you can set the PCB layer to be printed and also the display mode properties
of each object type on that layer. This determines how they will print (Full, Draft or Hidden
mode).

Figure 25 Layer Properties dialog


11.2 Setting Scale and Orientation and Printer Options
Choose the Setup Printer command in the File menu to display the PCB Print Options dialog
box shown.

Figure 26 Setting the printer options

11.3 Copying Print Preview to the Window Clipboard
You can copy the current Printout preview to the Windows clipboard by clicking on the Copy
icon on the Main toolbar or the Edit » Copy menu command. You can also save the image as a
Windows Metafile by choosing the File » Export menu command.

11.4 PPC Documents
The Print/Preview documents can be renamed and copied either the current Design folder or to
other folders. You can use a Print/Preview document with another design by copying it to the
appropriate folder and changing the PCB to be printed by choosing the Tools » Set Target
Board menu command.


12 CAM Manager
The CAM Manager gives you total control over the setup and creation of the manufacturing
output files, including Gerber, NC drill and pick and place. The setups are saved with the
design in a CAM Output Configuration document and can be modified at any time. CAM
documents can also be copied from one design to another, making it easy to transfer your
preferred output file configurations.
To create a new CAM document for the current PCB select the File » CAM Manager menu
command. A blank CAM document is created, and the Output Wizard will automatically start.
Using the Wizard you can create an Output Setup for each type of output.
CAM Manager supports the following outputs:
• Bill of Materials
• DRC
• Gerber
• NC Drill
• Pick and Place
• Test Point Report

You can add a new Output Setup to your CAM Output Configuration document from the
Editor menu or by right clicking in the document editor window. Once an Output Setup is
created, it can be edited by double-clicking on its entry in the list of Output Set-ups.


CAM Outputs are generated by:
• Generate CAM Outputs button on the Main toolbar
• The Tools » Generate CAM Files menu command
• F9 function key
The data is output into appropriate documents in a CAM folder within the same folder as your
PCB file. The name is determined by settings in the CAM Options dialog box that is displayed
by choosing the Tools » Preferences menu command.


12.1 Bill Of Materials
This option produces Bill of Materials reports (Parts Lists). Double-clicking on a Bom Output
Setup displays the Bill of Materials Setup dialog box shown. Output format options are Text,
CSV (Comma Separated Variables) and Spreadsheet.

12.2 DRC
This option produces a Design Rules Check report. Double-clicking on a DRC Output Setup
displays the DRC Setup dialog box shown.


12.3 Gerber
This option produces a Photoplotter output in Gerber format. Double-clicking on a Gerber
Output Setup displays the Gerber Setup dialog box shown.

Consult your PCB manufacturer for their preferred settings.

12.4 NC Drill
This option produces a NC drill output in an industry standard format. Double-clicking on a
NC Drill Output Setup displays the NC Drill Setup dialog box shown.

Consult your PCB manufacturer for their preferred settings.


12.5 Pick and Place
This option produces component data that is used to program a Pick and Place machine.
Double-clicking on a Pick Place Output Setup displays the Pick and Place Setup dialog box
shown.

12.6 Test Point Report
This option produces information on the location and size of Testpoints for use in fabricating
test fixtures and programming testers.

Double-clicking on a Testpoints Output Setup displays the Test Point Setup dialog box shown.


13 3D Viewer
The 3D Viewer allows you to generate a 3D model of your PCB that you can view from any
angle. This enables you to visualise what the PCB will look like.
The benefits of the tool are to help locate design errors very early in the design process. Some
examples are:
• Component placement problems
• Mechanical interference problems
• Assembly problems

To run the 3D Viewer, click on this button on the main toolbar.

The 3D Viewer has a separate tab from the PCB Editor. A 3d view of your PCB displays is the
editor view and you can control you view of the PCB from the Browse PCB3D tab of the
Design Manager panel.
To model components in 3D, 3D Viewer uses a run-time component modelling algorithm that
uses the component designator prefix, footprint and outline shape to automatically select
model and texture information and construct a suitable component model. Components that
cannot be recognized are automatically extruded.


Options for the 3D Viewer are set using the View » Preferences menu command in the 3D
Viewer. This displays the Preferences dialog box shown.

To change the view of the PCB you position the cursor in the MiniViewer in the Browse
PCB3D tab of the Design Manager panel. You then click and hold and move the cursor to
rotate the viewer of the PCB.
A Highlight net function is provided that allows you to see tracks belonging to selected nets.
Choosing Animated Highlighting in Preferences causes the selected tracks to “pulsate”.


14 PCB Library Editor
The PCB Library Editor is provided to create and modify PCB components and manage PCB
component libraries. In addition to enabling you to build components as required, it also
provides a Component Wizard to guide you through the creation of most common PCB
component types.

14.1 The PCB Library Workspace
The PCB Library editor workspace is shown below.

Figure 27 PCB library Editor Workspace

The view commands, primitive objects, layers, selection and focus, grids and general editing
functions are all identical to the PCB editor.
Also, settings in the Preferences dialog box and Document Options dialog box also apply in
the PCB Library editor.


14.2 PCB Library Editor Panel
The PCB Library Editor panel provides a number of
facilities for working with PCB components. These
are described below:
Component Section
The top section of the panel comprises a scroll box
that lists all the components in the active library. The
Mask field allows you to selectively list components.
The buttons at the bottom of component list do the
following:
< Move the cursor up one
component in the list
<< Move the cursor to the top of the
list
>> Move the cursor to the bottom of
the list
> Move the cursor down one
component in the list
Rename Renames the selected component
Place Places the selected component
into the active file in the PCB
editor
Remove Deletes the selected component
from the library
Add Creates a new component and
launches the Component Wizard.

The scroll box in the lower part of the components
section lists the pin numbers of the pads in the
selected component.
Click on a pin number to select it and then click on the Edit button (or double-click on the pin
number text) to display the Change Pad dialog box.
Click on the Jump button to zoom in on the selected pad in the display window.
The Current Layer Section displays the current layer and allows you to change the current layer
by clicking on the down arrow.


14.3 Creating a Component Using the Component Wizard
The PCB Library editor includes the Component Wizard. This Wizard allows you to select the
component category and fill in appropriate information and then builds the component for you.
To launch the Component Wizard press the Add button on the Library Editor panel or select
the New Component menu item in the Tools menu.

14.4 Manually Creating a Component
Components are created in the PCB Library Editor using the same set of primitive objects
available in the PCB Editor. In addition to PCB components, corner markers, phototool
targets, mechanical definitions etc can be saved as components.
The typical sequence for manually creating a component footprint is:
Open the desired library in the Library Editor.
Select the Tools » New Component menu command. The Component Wizard will
automatically start, press Cancel to manually create a component. You will be presented with
an empty component footprint workspace, called PCBComponent_1. Select Tools » Rename
Component to change this to the required name. Component names can be up to 255
characters.
Use Tracks or other primitive objects to place the component outline on the Silkscreen layer.
Place the pads according to the component requirements. When a pad is floating on the cursor
select Edit » Jump » Reference to position the cursor at the workspace 0, 0 coordinate. Prior to
placing the first pad, press the Tab key to define all the pad properties. Make sure you set the
Designator property correctly. Typically, the first pad you place is pin 1 so the set designator to
1 for the first pad. The designator automatically increments.

14.5 Copying a Component
There is often the requirement to copy components, either from one library to another or
within the same library. To achieve this use Edit » Copy Component. This copies any
components that are selected in the Components list in the editor panel to the Clipboard. To
select a component, click on the name text of that component. To select additional
components, use Ctrl+Click.
You then use Edit » Paste Component to paste components on the Clipboard into the active
PCB Library document.

14.6 Special Strings in the Library Editor
There are two special strings that are active in the library editor which are provided to allow
you to control the positioning of the Designator and the Comment.
These special strings are:
.Designator
.Comment


Place these in the PCB Library editor workspace at the location relative to the component
where you would like the designator or comment to be placed.
When you use these, you can hide the default designator and comment that are added when the
component is placed in the PCB file.

14.7 Component Rule Check
The Component Rule Check command in the Reports menu allows you to check either the
current component or the whole Library for any of the following:
• Duplicate pads
• Duplicate primitives (i.e. identical objects at the same coordinate)
• Duplicate component names
• Missing pad designator
• Bottom layer components
• Reference outside component objects
• Shorted copper
• Unconnected copper
The results of the component rule check are displayed in a text document.

14.8 Exercise – Libraries and Components
1. Create a new library file using File » New.
2. Create a new component of your choice using the Component Wizard (use Tools » New
Component).


15 Short Cut Key Summary
L Layers Tab of Document Options
Q Toggle Units
PgUp, PgDn View » Zoom In, View » Zoom Out
CTRL+PgUg/PgDn Zoom maximum / minimum
SHIFT+ PgUg/PgDn Zoom at 0.1 step rate
HOME View » Pan
END View » Refresh
CTRL+HOME Jump Absolute Origin
CTRL+END Jump Current origin
CTRL+INS Edit » Copy
CTRL+DEL Edit » Clear
SHIFT+INS Edit » Paste
SHIFT+DEL Edit » Cut
ALT+BACKSPACE Undo
CTRL+BACKSPACE Redo
SHIFT+F4 Cascade Windows
SHIFT+F5 Tile Windows
* Toggle active signal layers
+ or - Next / previous active layer
F1 Help Index
Popup Menus
A Tools » Align submenu
B View » Toolbars submenu
G Snap Grid popup menu
J Edit » Jump submenu
M Edit » Move submenu
O Options popup menu
S Edit » Select submenu
U Tools » Unroute submenu
X Edit » DeSelect menu
Z Zoom popup menu


Interactive Routing
BACKSPACE Removes the previously placed track segment while routing a
connection.
* Toggles through the routing layers while routing.
/ Places a via connecting to a power plane.
TAB Pop up the Track properties dialog box to edit track attributes
while routing.
SHIFT+R Cycles through the interactive routing modes.
SHIFT+S Toggles single-layer display mode on and off.
SPACEBAR Changes between track placement start and end angle modes.
SHIFT+SPACEBAR Cycles through the track placement modes.
CTRL+SPACEBAR Cycles through the connection lines connecting to a pad.
CRTL Temporarily suspends the electrical grid.
ALT Temporarily switches from Avoid Obstacle to Ignore Obstacle
mode.
End Refreshes the display while routing.
Useful Information
Protel Website www.protel.com
Protel User Group PROTELEDAUSERS@techservinc.com


Protel 99 se_traning_manual_pcb_design

More Related Content

What's hot (7)

Similar to Protel 99 se_traning_manual_pcb_design (20)

Recently uploaded (20)

Protel 99 se_traning_manual_pcb_design