Moving to Altium Designer from PADS

MOVING TO
ALTIUM DESIGNER
FROM PADS



Tool-chains vs. Altium’s Platform Approach

To remain competitive, companies must continuously strive to improve engineering
design methodologies and process improvements aimed at reducing overall
development cycles and minimizing costs. In order to achieve these goals, when making
the decision to switch out your current EDA tools, protecting your investment in your
schematics, PCB designs and library data is an important factor to consider.

The traditional approach to delivering EDA tools has been focused on providing best in
class point tools, independent processes that are interfaced along the tool chain which
inherently requires multiple learning curves for the different tools. Altium Designer
delivers a unified design environment that provides a single user interface, from
schematic capture, PCB layout, Library management and design data management
with version control through to integrated FPGA and Embedded software development,
which ultimately results in improved productivity and efficiency.

A scalable solution set addresses the requirements of the individual designer, small and
large design teams and the company IT infrastructure. Design and tool configuration
management and an integrated Vault based design data management system ensures
that the entire ECAD design flow is supported, from conceptual design, component and
part creation, work-in-progress, release to manufacturing and the ECO process.

Integrated 3D PCB editing with Flex-Rigid design capabilities, automated 3D clearance
checking and STEP model support solves another of the tool chain based challenges by
bringing the ECAD and MCAD domains closer together to ensure that complex PCB
structures and their components actually fit in the desired packaging.

Access to the extensive Design Content library, currently in excess of 200K part/
components is provided through the AltiumLive user portal. Library content is regularly
updated and new parts are created from vendor data sheets and include everything you
need to start, finish and build a design, including Schematic symbols, PCB footprints,
3D models and parametric data linked directly to supplier’s web sites to ensure that
the most up to date part information including availability and cost is available to the
designer throughout the design cycle.

This document guides you through the process of moving from PADS to Altium
Designer.

MOVING TO ALTIUM DESIGNER FROM PADS 2

Smooth transition from PADS to Altium Designer

Translating complete PADS® designs, including PADSLogic™ schematics, PADSLayout™
PCB files, and library files can all be handled by Altium Designer’s Import Wizard.
Therefore, migration from PADS to Altium technology is a straightforward process with
Altium Designer’s unified data and file translation features. The Import Wizard
removes much of the headache normally found with design translation by analysing
your files and offering many defaults and suggested settings for project structure,
layer mapping, PCB footprint naming, and more.

Altium has created extensive systems and features within Altium Designer to make the
task of successfully transitioning from other systems as easy as possible, with a minimum
of disruption to productivity. As a result our highly-developed Wizard-based design
file translators guide you through the import process for all design documents –
including libraries – while managing the relationship between them. Complete
flexibility is found in all pages of the Wizard, giving you as little or as much control as
you would like over the file translation settings, before committing to the actual
translation process.

Altium Designer’s translators import all documents in one operation and include
specific support for PADS design and library files. With a series of simple, interactive
steps the Import Wizard processes all file types to automatically create ready-to-use
Altium Designer projects and integrated library files, while accurately processing
essential design elements such as polygon pours, text positioning, design rules, and
layer mapping.

The translation features include:

• Import Wizard to smoothly guide you through the import process

• Batch import of multiple projects for rapid migration of large sets of design
data

• Import engines intelligently handle translation and object mapping

MOVING TO ALTIUM DESIGNER FROM PADS 3

Supported versions and file formats 4

Altium’s Import Wizard can translate PADS schematic, layout and library data. However,
all data must first be exported from PADS as ASCII data. PADS Logic and PADS Layout
both have File»Export menu selections for this. ASCII export of library data is done in
the PADS Library Manager. First choose the desired library type (Decals, Parts, Logic),
then select which items are to be exported, then click the Export button. Decal libraries
will export to a .D file, Parts will export to a .P file and Logic (CAE) will export to a .C
file. The following file formats are supported:

• PADS Layout/PowerPCB ASCII (*.ASC) files up to and including V9.3
• PADS PCB Decal Library ASCII(*.D) files
• PADS Logic/PowerLogic ASCII (*.TXT)files up to and including V9.3
• PADS Schematic Part and CAE Decal Library ASCII Parts (*.P + *.C)
Schematic and PCB files translate as follows:
• PADS Layout/PowerPCB ASCII (*.ASC) files translate to Altium Designer

PCB files (*.PcbDoc)
• Schematic sheets within a PADS Logic/PowerLogic ASCII file(*.TXT)

translate to Altium Designer Schematic files with a *.SchDoc file
extension. Each schematic sheet will create a separate .SchDoc file.
• These files will be grouped into an Altium Designer PCB project (*.PrjPCB)
that is automatically created
• See the topic “Component Linking through Unique IDs” at the end of
this document for details on linking files together to allow for cross-
navigation and ECO generation.

Library files translate as follows:
• PADS Schematic Library ASCII (*.C+*.P) files will be combined into
Altium Designer Schematic library files (*.SchLib). The .C file contains the
graphical portion of a schematic component, and the .P file contains the
specific part information (pin information, default reference designator,
parameters/attributes, footprint/decal pointers, etc.).
• PADS PCB Library ASCII (*.D) files translate to Altium Designer PCB library
files (*.PcbLib)

• Translated PADS libraries are automatically grouped into one PCB project.

MOVING TO ALTIUM DESIGNER FROM PADS

Using the Import Wizard for PADS Files

The Import Wizard can be launched from the Altium Designer File menu. Choose the
PADS ASCII Design And Library Files option as shown in Figure 1.1 On the “Importing
PADS Designs” screen, click the Add button to choose Layout and/or Logic files. Use
the filter button at the bottom right of the file browser to switch between .ASC and
.TXT files. Multiple files can be translated at the same time. Step-by-step instructions on
using the Import Wizard follow at the end of this document.

Figure 1.1 Starting the Import Wizard for PADS files

Options for PCB Files

The Import Wizard presents users with several options to control the translation from
PADS to Altium Designer, including which sets of design rules come across, and how
keep-outs are handled. Refer to Figure 1.2 for those options. Take special note that
the all options are enabled, including “Generate Teardrops” which will add teardrops
to pads and vias upon design translation. Disable this option if your design does not
require the use of teardrops.

MOVING TO ALTIUM DESIGNER FROM PADS 5

Figure 1.2 Translation Options

Layer Mapping for PCB files

PADS PCB files will be analysed before translation to best determine how layer
definitions in PADS will be mapped to Altium Designer layers. Efforts will be made
to ensure, for instance, PADS silkscreen layers map to Altium silkscreen layers. Layer
mapping can be manually adjusted if desired. In addition, PADS layers can be set
to “Not Imported” if information from a particular layer can be discarded. Specific
to internal layers, PADS inner signal layers will be initialised as Altium signal layers
(e.g., “Mid Layer 1”). PADS CAM Plane layers will be initialised as Altium Plane Layers
(e.g., “Internal Plane 1”), which are negative-image planes similar to PADS CAM
planes. PADS inner layers defined as Split/Mixed layers will be initialised as Altium
signal layers if any trace or other positive image electrical data is present. If the Split/
Mixed layer only has pour shapes it will be initialised as an Altium Plane layer, and
imported with all split, embedded, and isolated plane areas intact. This setting, as
mentioned, can be changed manually by the user.

PADS PCB files and PCB Decal library files in both the default 30 layer mode and the
expanded 250 layer mode are supported. If the default layer mappings are customised
by the user, those setting can be saved to a configuration file so that those mappings
can be quickly reused for subsequent translations.

MOVING TO ALTIUM DESIGNER FROM PADS 6

Working with schematic documents

In PADS Logic there can be multiple schematic sheets within a single schematic design
file (*.SCH file). In Altium Designer, each schematic sheet is a separate document.
This means that for each Altium Designer schematic sheet there is a file (*.SchDoc),
an important conceptual difference to remember. All schematic documents are then
grouped together in a Project file (*.PrjPCB) to establish sheet-to-sheet connectivity.

There can also be multiple design documents of varying types, depending on the nature
of the design you are working on. Getting started, most PADS users will be interested
in the schematic and PCB document types as these are the files that their designs will
be translated to.

New schematic and PCB document types can easily be created via the File»New menu,
or by right-clicking on the project in the Projects panel and selecting Add New to Project
from the floating menu.

Workspace Panels

Many elements of the environment will appear intuitive to PADS users, helping as you
to start exploring the system. For example, the Projects panel will appear similar to the
PADS Logic Project Explorer view, except that it is not limited to schematic design data
and can include the PCB, all libraries, output files, as well as other project documents,
such as MS Word or Excel files.

Figure 1.3 Figure 1.3. Project Explorer view 7
in PADS Logic showing a 4 sheet schematic.

Figure 1.4 Projects panel in Altium Designer show-
ing a 4 sheet design, plus corresponding PCB design
and libraries.

MOVING TO ALTIUM DESIGNER FROM PADS

Defining Net Connectivity 8

In PADS Logic, net connectivity is made using direct connections, net name labels, and
power/ground/off-page symbols.

Altium Designer uses a similar set of net identifiers to create net connectivity. Within
a schematic sheet you can use Wires and Net Labels. Between schematic sheets, nets
in a flat design are typically connected using Ports, but Off-Sheet Connectors are also
available in purely flat designs. Nets in a hierarchical design are connected from a
Port on the lower sheet to a Sheet Entry of the same name, in the sheet symbol that
represents the lower sheet. Power/ground nets are connected using Power Ports.

Working with PCB Files

Translated PADS Layout files will retain all of the electrical information from the original
PCB file: decal (footprint) definitions, all routes and vias, net names, etc. There may
be areas, however, that may warrant some inspection by the user. Polygon (copper)
pours are defined slightly differently than in PADS and have their connectivity and
clearances driven by Design Rule settings rather
than by properties or preferences. Go to the
Design»Rules menu and inspect the “Polygon
Connect Style” rules found in the “Plane” section
to view and change polygon pour connectivity.
Polygon Pours may then need to be repoured to
maintain design intent. Keepout areas are also
defined differently in Altium Designer and should
also be inspected.

Figure 1.5 Polygon Connect Style rule
category in Design Rules

The Altium Designer Environment

Main article: The Altium Designer Environment, Altium Designer Panels

The Altium Designer environment offers a complete electronic product development
environment for all areas of design - from schematic capture to the generation of PCB
output, as well as complete FPGA design, development and on-chip debugging.
The environment is fully customisable, allowing you to set up the workspace to suit
the way you work. Consistent selection and editing paradigms across the different
editors allow you to easily switch between various designs tasks all within the Altium
Designer environment.

MOVING TO ALTIUM DESIGNER FROM PADS

Perhaps the single biggest difference that you will notice when you start working in
Altium Designer is that there is only one application used to create and edit all design
files, regardless of the type of file - schematics, PCB, library, text, and so on. No longer
will you have to switch between different applications when you want to move from
viewing the schematic to the PCB. All the files (also referred to as documents) open
in the same executable, each appearing on a separate Document Tab within Altium
Designer. As you move from one type of document to another the menus and toolbars
automatically switch, giving you the right editing environment for that document.

Getting Help

Main article: Documentation and Help

• F1 over any object, editor, panel, menu entry or button to open a brief
description in the Knowledge Center panel.

• Shift+F1 while running a command for a list of shortcuts you can use in
that command.

• Search Altium Documentation

• Visit the Altium Video Library where you can watch over 100 short
training videos, each detailing the exact steps needed to complete a
task.

AltiumLive

In AltiumLive you can share all your thoughts with your industry peers. It is the central
place for users of Altium. This includes a complete Ecosystem to deliver content,
knowledge and experience of other users to you. Also, it is a place where you have a
direct interface to Altium for any feedback like a feature request. With that feedback,
we are much better prepared to improve our software in a way the market really
requests.

• Content: You will find content like libraries, design secrets and
reference designs

• Forum: Discuss your topics with Altium staff and users.

• Blogs: What’s new, technical and commercial topics around Altium.

• BugCrunch: Report Bugs, request features and vote for implementation

MOVING TO ALTIUM DESIGNER FROM PADS 9

Project-Based Design

Main article: Project Management

The starting point for every design created in Altium Designer is a project file. There are
a number of project types supported, each targeting a different final implementation,
for example PCB project, Library project, FPGA project, Embedded project, Core Project
and Script project. The project file stores links to the actual design documents that are
part of the project, as well as project-specific settings. Using this concept, you have
additional possibilities like defining rules for PCB design already in Schematic. Also, this
is a central storage place for your complete design, e.g. for the design rules.

Multi-Channel Design

Main articles: Multi-Channel Design Concepts, Creating a Multi-channel Design

There are several multi-channel reference designs available. These include the Multi-
Channel Mixer, Peak Detector and Port Switcher. All three designs can be found
within AltiumLive. Once you have opened one of the examples you should compile it,
and then look for the compiled document tabs at the bottom of the schematic editor.

Complex hierarchy is the general term used throughout the industry to describe
the process of using multiple instances of the same sheet in a schematic hierarchy.
Traditionally, a design that included complex hierarchy had to go through a process
of ‘flattening’ or ‘expanding’ the hierarchy at some point, to uniquely instantiate
every component and net. Altium Designer does not need to do this, so this multiple-
instantiation capability is referred to as multi-channel design instead of complex
hierarchy.

The ability to be able to make each channel different by passing parameters to it from
the parent sheet symbol is also supported, and is referred to as parametric hierarchy.

Using parametric hierarchy you can parametrically define the component value,
supporting the situation where a component does not have the same value in each
channel. Parametric components are defined by declaring their value as a parameter of
the sheet symbol above, and then referencing that parameter on the target component.

MOVING TO ALTIUM DESIGNER FROM PADS 10

Preferences

Main article: Altium Designer Environment Preferences

Global Preferences are accessed by selecting DXP»Preferences from the menus. The
preferences configured here are stored as part of your installation, they do not travel
with the design files. File-specific settings, such as schematic document options and
printed circuit board options are accessed via the Design menu in each editor.

PCB Layout and Design

Successful board layouts rely on design systems that unify the design definition with the
physical layout and routing. Altium Designer offers such a PCB system which includes
a number of familiar features to help you place and route your board. When the PCB
Editor is active (i.e,. a PCB document (*.PcbDoc) is open and active) the main application
window will contain:

• A main design window in which you can start designing, capable of
display in both 2D and 3D (shortcut: 2, 3)

• Menus and toolbars that are specific to the PCB Editor

• Workspace panels that are both global and editor-specific

View Configuration and the Layer Stack Manager

View Configurations are settings that control many PCB workspace display options for
both 2D and 3D environments, and apply to the PCB and PCB Library Editors. The view
configuration last used when saving any PCB document is also saved with the file.

Select Design»Board Layers & Colors (shortcut: L) from the main menu to open the
View Configurations dialog, or switch configurations using the drop down in the main
toolbar, as shown below.

Figure 1.6 The Layer Stack can be easily managed and copied to the Clipboard 11
for documentation purposes.

MOVING TO ALTIUM DESIGNER FROM PADS

To open the Layer Stack Manager select Design»Layer Stack Manager (shortcut D, K) 12
from the menus. The Layer Stack Manager dialog shows the current layer stack up of
the board. Signal and plane layers can be added, removed, or their order changed.
Double-click on an electric or insulation layer to configure layer properties, such as:
thickness, net association (plane layers), or the dielectric constant.

PCB Board Options - Document Settings

All options for the placement grid, measurement units, sheet position, and designator
display mode are set in the Board Options dialog. With a PCB document active in the
main design window (for this and all of the following context-sensitive dialogs), select
Design»Board Options (shortcut D, O) from the menus to open the Board Options
dialog.
For multi-channel designs, you can select between logical and physical designator
display on the PCB in the Board Options dialog.

PCB Board Wizard

Before you can transfer your design from the Schematic Editor to the PCB Editor, you’ll
need to have at the very least a blank PCB with at least a board outline. The PCB Board
Wizard allows you to easily create a basic PCB design using many industry-standard
board outlines as well as create your own custom board sizes. The PCB Board Wizard is
launched from the Files panel in the New from template section. At any stage you can
use the Back button to check or modify previous pages in the wizard.

Interactive Routing

Main article: PCB Routing
Altium Designer also has different interactive routing modes for interactive routing
for single tracks, differential pairs and busses. Modes for interactive routing are not
dependent on licensing options, and are all available in the PCB Editor with different
routing obstacle avoidance modes:

• Ignore obstacles
• Push obstacles
• Walk around obstacles
• Stop at first obstacle
• Hug and push obstacles
• Follow mouse trail

MOVING TO ALTIUM DESIGNER FROM PADS

Design Rules

Main article: Design Rules

Altium Designer’s PCB Editor is a rules-driven design environment. You can also
transfer your favourite design rules from another board. Design rules can be exported
from, and imported to, the PCB Rules and Constraints Editor dialog.

Figure 1.7 The PCB Rules and Constraints editor in Altium Designer can be opened in the PCB Editor with
the Design > Rules command.

Signal Integrity

Main articles: Performing Signal Integrity Analyses, Signal Integrity Analysis,
Signal Integrity Rules, Signal Integrity Panel

In addition to the standard set of design rules for DRC, Altium Designer also supports
Signal Integrity analysis, which is integrated directly into the PCB Editor (Tools»Signal
Integrity). This includes:

• Pre-layout and post-layout Signal Integrity analysis capabilities that you
can perform from either the Schematic or the PCB Editors;

• Evaluate net screening results against predefined tests
• Perform reflection and crosstalk analysis on selected nets, and display

waveforms
• Calculate suitable termination values using the termination advisor for

different termination topologies
• Impedance driven routing, as well as support for balanced differential

pairs
• Length tuning by adding accordions to your single ended and differential

pairs

MOVING TO ALTIUM DESIGNER FROM PADS 13

Mixed-signal Circuit Simulation 14

Main article: Circuit Simulation

Mixed-signal circuit simulation is a unified part of the capture process, and is
fully integrated with the schematic editing environment. Before you launch the
Mixed-signal circuit simulation, make sure that any schematic sheet within the
project is open. Simulation models need to be associated with every component
in the schematic document before simulation can be launched from the command
Design»Simulate»MixedSim. Simulation is done for the entire project.

You can use the same Schematic for both: Simulation and PCB because of Altium
Designer’s unified data model. This integrated simulation environment is fully SPICE
compatible and additionally supports PSPICE models.

See Also for PCB Design

• A great place to start learning about PCB Design is Tutorial - Getting
Started with PCB Design

• Editing Multiple Objects to learn about editing using the Find Similar
Objects functionality

• PCB Inspector Panel which displays the common properties of different
objects and lets you filter and edit them

• Editors, Panels and Object Reference to learn more about the PCB
Environment

• Preparing the Board for Design
Transfer

• Situs Autorouting Essentials

Compilation - a Cornerstone of Altium Designer

Compilation is a cornerstone concept of the Altium Designer environment. Compilation
is a process that allows you to harness many powerful design features.

When you complete your PADS schematic design, you are used to generating a netlist
and importing this insufficient information into your PCB tool. With Altium Designer
you do a compilation instead. With that you transfer any available information into the
unified database for your project. From here, it is available to any other domain available
inside this powerful toolset. For the transfer of data from one domain to the other
Altium Designer will offer you an engineering change order process (ECO). With that
ECO, you have full control over what should be transferred.

MOVING TO ALTIUM DESIGNER FROM PADS

When you select Project»Compile Project the compilation process works out the
structural relationships between the source schematic (or HDL) documents in the
project, then determines the net-level connectivity within each sheet, and finally the
connectivity between the sheets. All this component and connective intelligence from
your schematics design is written into Altium Designer’s unified internal data structure
that can then be used for many post-compilation activities, such as comparing and
showing differences between schematics, parameter managing, parametric navigation
of your design, cross probing back and forth between the schematics and PCB, and
much more.

Where are my nets and components from my design?

Connectivity is not as explicit in your design as it was before, but rather has to be
extracted from the design using the compilation process. This is available through the
right-click menu in the Projects panel, or using the Project»Compile Project menu
command.

Once the design is compiled the sheet-level hierarchy, as well as all the components,
nets and buses are displayed in the Navigator Panel. From here you can easily locate any
component, bus, net or pin throughout the entire design. And if you hold the Alt key as
you click on an object in the Navigator Panel it is highlighted on the PCB as well as the
schematic – no longer will you need to inspect net lists to review design connectivity.

Configuring Design Connectivity

Main article: Connectivity and Multi-Sheet Design

Altium Designer supports different types of design connectivity, and this must be set
to suit the structure of the design. The type of sheet-to-sheet connectivity is called the
Net Identifier Scope. This is defined in the Options tab of the Options for Project dialog
and saved with the project. From the Project menu select the Project Options menu
command, and go to the Options tab.

MOVING TO ALTIUM DESIGNER FROM PADS 15

Figure 1.8 The Net Identifier scope is set in the Options tab of Project Options 16

In the Net Identifier Scope dropdown you can select from the following connectivity
options:

• Automatic (Based on project contents)
• Flat (Only ports global)
• Hierarchical (Sheet entry <-> port connections)
• Global (Net labels and ports global)
The Import Wizard handles connectivity automatically through the translation process
and will give you the Automatic (Based on project contents) configuration by default.
Hierarchical blocks are mapped as sheet symbols, and they will translate to sheet
symbols in Altium Designer. In Automatic mode, the design compiler then looks at the
sheet symbols on the top sheet. If there are sheet entries (hierarchical pins) in them,
it will assume vertical connectivity, and internally use the Hierarchical option. If there
are no sheet symbols on the top sheet, or if there are sheet symbols but they do not
include any sheet entries, it will assume horizontal connectivity for which there are two
ways that Altium Designer supports this: Flat and Global. In order to determine which
of these two options to use, the design compiler looks for ports or off-sheet connectors
on the subsheets. If there are any it uses the Flat option, if there are no ports it uses the
Global option.
You can easily go back and change the configuration after translation through the
Project Options dialog from the Projects menu.

MOVING TO ALTIUM DESIGNER FROM PADS

Verifying Your Design - Expanded Error Checking

Main articles: Project Compiler Error Reference, Compile Errors Panel

Another benefit that results from compiling a project in Altium Designer is built-in
error reporting. This is completely configurable for your needs and can be done before
your project is compiled. Right-click either on the project file and invoke the Project

Options command, or also through the Project menu.

Design Synchronization

Main article: Finding Differences and Synchronizing Designs

Design synchronisation is fully integrated in Altium Designer without the need for
passing a net list. Synchronisation in Altium Designer is also bi-directional, allowing
you to make annotation changes and component property updates in both directions
between your schematic and PCB, in a single operation.

Components and Libraries

Main article: Component, Model and Library Concepts

Altium Designer supports working directly from the source symbol or model libraries,
an ideal approach when the schematic and PCB are designed by separate
organisations.

The logical symbol is assumed to be the essential starting point of a component. It can
be initially defined at minimum as a name in a schematic library to which pins and any
graphical symbols or alternative display options needed for implementation may be
added. This flexibility allows a component to be represented in different ways during
the design and capture process. This may not only be as a logical symbol on the
schematic, but also be a footprint on the PCB or even as a SPICE definition for
simulation.

With Altium Designer a new model is available: Component Libraries, where any
component is unique, life cycle managed and version controlled available from your
company vault and linked to your company database. With part choices, you can
leverage the existing know how from your design teams with the knowledge of the
purchase department. E.g. a part becomes obsolete, or your designer allows the
purchaser to use a 1% resistor instead of a 5% if he buys this in higher quantities.
With the relational database you will immediately see where and how often
this part has been used in your company.

MOVING TO ALTIUM DESIGNER FROM PADS 17

Where are my libraries?
Some Basics on Library Management

You’ll be able to view your source schematic and PCB library files immediately after
translation through the Projects panel. Your translated libraries are automatically
grouped into one PCB project.

Libraries are installed (added) to the Altium Designer environment, making their
components available in all open projects. Display the Libraries panel, from there you
can install and remove libraries. Libraries can also be linked to any project, and you can
also define project search paths, useful for referencing simulation models.

See Enhanced Library Management Using Integrated Libraries for a further discussion
on using Integrated Libraries.

A Brief Note on Database Linking

Main article: Linking Existing Components to Your Company Database,

Appreciating the fact that many designers like to link from the components in their
electronic design software to their company database, Altium Designer has strong
support for linking and transferring database data through the design process and into
the Bill of Materials.

Two techniques are supported, one where the Altium Designer library symbol holds
all model references and also includes links into an external database, the second
where the database holds all model references and other company information. While
database connections in Altium Designer are set up for MS Access databases (*.mdb
files) by default, any ODBC-compliant database can be accessed.

MOVING TO ALTIUM DESIGNER FROM PADS 18

Multiple Monitor Support

Altium Designer has full support for multiple monitors. If you have multiple monitors
on your PC you can easily drag a document or Workspace panel out of Altium Designer
and drop it on the second monitor, greatly enhancing your design productivity. Multi-
monitor support is configured in Windows.

Project Outputs

Generating documentation has always been an essential part of your work. If you want
to automate your design outputs and therefore make it repeatable, you can leverage
this by using the concept of Output Jobs. Output Jobs are a graphical way to batch
all of the settings necessary to generate any output. If you have defined them once,
generating all of the necessary files with all of the necessary settings is just one mouse-
click away. And if you implement them into your new document defaults, generating
outputs for your next projects will also be one button push away. In Altium Designer
output jobs are the basis of our release data management. With that you can
standardise your complete release management and make it a push-button solution
to make it right the first time.

To learn about generating manufacturing output, either using the OutputJob Editor or
using the Reports menu see Design to Manufacturing

To learn about the CAM Editor see Auto-Loading Fabrication Output into the CAM
Editor

To learn about the built in PDF generation wizard, see Smart PDF available from the
File menu.

MOVING TO ALTIUM DESIGNER FROM PADS 19

Step-by-Step Import Instructions

In the following step-by-step instructions, the “Preview” schematic and PCB design files
coming from the PADS “Samples” directory will be used.
• Start the Import Wizard with File»Import Wizard

Select Type of Files to Import—>PADS ASCII Design And Library Files

MOVING TO ALTIUM DESIGNER FROM PADS 20

• Add the file(s) to be translated. In this case, the “preview.txt” (Logic) and “preview.
asc” (Layout) are used.

Note: You can add as many .txt and .asc at this point.
Note: In the file browser, change the file types pull-down to choose .asc or .txt files.

In the next step you can add your Schematic or PCB Libraries to import (if available)

Note: Because the library part and decal information is included in the source files, it is
not necessary to add libraries for schematic or PCB files to successfully translate. Only
add libraries to this screen if you wish to independently translate entire libraries for later
use in Altium Designer.

MOVING TO ALTIUM DESIGNER FROM PADS 21

• Set the options for what level of reporting is done after the translation has completed.

MOVING TO ALTIUM DESIGNER FROM PADS 22

• Set the option to simplify imported padstacks by using the largest pad found for all
layers.

• Set PCB Options, for instance, which PADS design rules are to be translated, how
PADS keepouts are to be converted, etc. The “Generate Teardrops” option will
add teardrops to the PCB design, so do not enable this if teardrops are not needed
in your design.

MOVING TO ALTIUM DESIGNER FROM PADS 23

• Click the Edit Mapping button to configure which layers are converted and what
layer types they are converted to.

• The PCB file will be pre-analysed to determine what the PADS layers are and initialise
the layer mappings so that, for instance, the PADS silkscreen layers convert to Altium
silkscreen (overlay) layers.

MOVING TO ALTIUM DESIGNER FROM PADS 24

Note: PADS Split/Mixed layers will be analysed to determine if the layer is being used
as mixed layer (i.e., has pour AND route data) or as a split plane layer (just pours). If
the latter, the layer will be initialized as an Altium Plane (which is a negative layer) to
take advantage of Altium’s split plane capabilities. If you wish the S/M layer to remain
a positive image pour layer, remap the layer to one of Altium’s “Mid Layers” which are
positive. In the “Preview.asc” example, the Power Plane layer has only pours for the
+5V and +12V nets but no routes, so it is initialised as an Altium Plane. For this
example, we will show it remapped to an Altium Mid Layer.

MOVING TO ALTIUM DESIGNER FROM PADS 25

• A preview of the files being translated and their output directories are shown.
Change the main output directory if desired.

MOVING TO ALTIUM DESIGNER FROM PADS 26

• Click the final Next button and the Import Wizard will take care of the rest.

• Open the translated Project files. After compilation of your design in Altium Designer
with Project»Compile Project your design has been successfully brought into Altium
Designer! A matching schematic and PCB will allow the use of the Cross Select Mode
by enabling Tools»Cross Select Mode in both the schematic and PCB editors.
Component selection in either editor will select the matching component in the other
editor. For more robust Cross Navigation and ECO capabilities, it is recommended that
the Component Links be synchronized. The next section details that procedure.

MOVING TO ALTIUM DESIGNER FROM PADS 27

Component Linking through Unique IDs

Altium Designer uses several methods to connect and synchronize data between the
schematic and the PCB. Component reference designators and net connectivity is one
way, but a more robust method is through the use of a Unique ID. This is essentially a
serial number that is given to a component when it is placed on the schematic, which
is then transferred to its corresponding footprint when the schematic data is brought
over to the PCB.

Figure 1.9 Unique ID field in schematic

Figure 1.10 Matching Unique ID field in PCB

This allows much greater flexibility in reannotating reference designators, as
previous synchronisation of the designators is not a requirement; the synchronisation
is all done via the Unique ID. The ECO process and other synchronization checks
can be done much more quickly and easily when the Unique IDs all match.
During a “normal” design process starting at the schematic then going to PCB, the
Unique IDs are automatically passed so it’s a transparent process for the user. For
translated files, however, the Unique IDs do not automatically get synchronised. Not
to worry – Altium Designer has a tool to do this for you!

MOVING TO ALTIUM DESIGNER FROM PADS 28

In the PCB editor, select Project»Component Links. The dialog will show (on the right
side) the components that currently have matching Unique IDs. Those in the left
and centre columns are unmatched:

Clicking the Add Pairs Matched By>> button will link the Unique IDs using various
methods – the simplest and default being reference designator matching. Components
whose reference designators match will then be placed in the Matched Components
column. Clicking Perform Update will change the Unique IDs in the PCB to match those
found in the schematic.

MOVING TO ALTIUM DESIGNER FROM PADS 29

See Also

A great place to start your journey through all of the new possibilities is with your
Altium Designer installation. On the top right of Altium Designer you can find the
Home button.

From here, you can easily access the Documentation Library in the Tasks area where
the “Getting Started with Altium Design Solutions” category will ease your start into a
unified future.

MOVING TO ALTIUM DESIGNER FROM PADS 30

All1um