Altium Evaluation Guide For Autodesk Eagle™ Users
THE ALTIUM DESIGNER PHILOSOPHY
The core principle of Altium Designer is a unified approach to PCB design. In implementing this approach, you’ll find that our tool differs from many of the more conventional alternatives currently available. There are a number of separate yet connected elements required to complete a successful PCB design, and our workflow brings them all together.
TOPICS IN THIS SOLUTION
As an existing EagleTM user, you’re likely used to having a tool enabling you to do schematic and PCB work in a basic way. But how do you solve today’s needs when it comes to high-speed design tasks or requirements from mechanical departments? And what about documentation? A set of gerber files is usually not sufficient: BOMs for procurement and production are necessary as well as documentation of the whole design for different parties with different needs. Of course those things can be done with third-party tools. Throughout our tenure in PCB design, the question we’ve always asked is this: Is that approach really effective?
When we first created Altium Designer, we wanted to create an experience that kept the engineer in complete control of their efficiency and workflow throughout the entire design process. Achieving this goal meant getting to the heart of the matter: what, exactly, does a complete PCB design experience entail for the everyday engineer? As part of our approach, we connected the following processes into a single interface:
- Schematic Capture
- Board Layout
- Design Data Management
- Rules and Constraints
- Bill of Materials
- Supply Chain Integration
- Engineering Change Management
- MCAD Collaboration
- Manufacturing Documentation
With all of these elements integrated into a single, all-encompassing interface, switching back and forth between tasks becomes as simple as selecting the appropriate file to work on in your design workspace. The interface then handles all the rest and provides the tools you need for the particular task at hand.
Our unified PCB design approach has continued to grow and evolve over 30 years of research and development. We’ve found it to be, quite simply, the most efficient way to design electronics. This philosophy extends not just to the individual engineer, but also to the entire design team.
Multiple engineers can all work on different aspects of the same project using the same interface, and no time is wasted translating design data back and forth between design environments.
We hope you enjoy your journey into the world of Altium Designer.
Before importing any EagleTM file, the first step is to make sure the EagleTM Importer has been installed. This can be done directly within Altium Designer, using the following steps:
- Open Altium Designer
- Select File » Import Wizard
- Select Next on the Welcome screen
The next screen, ‘Select Type of Files to Import’, lists the installed importers.
Altium Designer Import Wizard file type selection
During the Altium Designer installation process, you can choose which Importers and Exporters to install. The EagleTM translator should be part of the default installation.
If the ‘EAGLE Designs and Libraries Files’ entry is missing from the list as shown above, then follow these steps to add it:
- Select Get More Importers at the bottom-left corner of the Import Wizard dialog window. This will open the Extensions & Updates tab inside the Altium Designer environment.
Altium Designer Extensions & Updates section
- Select Configure on the right and scroll down to the Importers\Exporters section.
- Check the boxes next to EAGLE to enable the extension.
Enable the Eagle® importer in the Altium Designer Extensions & Updates section
- Scroll back to the top and select Apply. You will then need to restart Altium Designer to complete the installation.
- Select File » Import Wizard and confirm that the EagleTM Importer has been added.
With the importer added in Altium Designer, you are now ready to start preparing your EagleTM files for the import process.
The EagleTM Import Wizard for Altium Designer supports the XML file format which has been introduced in EagleTM V6.
NOTE: Schematic and PCB data in the EagleTM binary format (V5.x and older) can be converted to the XML format simplyby re-saving them in EagleTM V6.x and upwards. If you do not have this capability, please get in touch with your local Altium representative.
Select File (top left) » Import Wizard.
The Import Wizard dialog box will appear. Click Next to proceed.
Select EAGLE Projects and Designs in the Select Types of Files screen. Click Next.
Click Add to browse to the location of the .sch and/or .brd files you wish to import. The files will appear as shown in the figure below. Click Next to continue.
Adding Eagle .lbr library files is optional, click the Add button to select the library file(s) you wish to import. Click Next to continue.
- The Reporting Options page will enable/disable the settings for logging errors, warnings, and events, respectively. In the schematic settings, you will find several options to optimize the importers result:
Ports and Power Ports, which are common parts in EagleTM, can be translated to Altium Designer primitives.
With ‘Ignore Document Templates’ selected, the frames being used in EagleTM will be skipped in the import process setting you in the position to add those you have been designing in Altium Designer afterwards.
By default Altium Designer provides a basic sheet template If you did not define your own. ‘Hide Default Sheet Template’ prevents the usage.
If you have chosen previously to import libraries as well, the library settings can be adjusted to either be added to the PCB Project you are importing or imported individually as a Library Project. Click Next to continue.
The default project location for the import process is shown below. Click Next to continue.
Executing Import Process
- The Messages panel may appear, which provides an interactive listing of the error, warning and status messages produced during the import. We don’t need this list at the moment, but when cleaning up the Project later on it will be a big help in the schematic area.
The dialog box can be closed by clicking the X in the top right corner of the dialog box.
- If the translation process is successful, then the Wizard is complete. You can click to close it and start working on your translated Schematic designs in Altium Designer.
Click Finish to complete the import process.
CLEANING UP YOUR IMPORTED DESIGN - PROJECT MANAGEMENT
Although schematic and PCB are translated during the same Import Wizard session, the translations are run as separate processes. When schematic and PCB are translated, the resulting files will be placed into a project. In this example, the “Arduino_MEGA2560_ref” schematic and PCB were run through the Import Wizard at the same time and have been put into one project like you are used to in Eagle.
Working with project files imported into Altium Designer
For more information on projects, refer to Project Management within TechDocs.
Instead of using Reference Designators to synchronize the schematic and the PCB, Altium Designer uses a Unique ID value. This can be thought of as a serial number for each component.
When creating a design from scratch in Altium Designer, each component automatically receives a system-generated Unique ID within the schematic editor.
When the design is transferred to the PCB editor, that Unique ID is passed over and resides on the corresponding footprint within the PCB document. In the example below, ‘IC3’ is assigned the Unique ID “BMYDMPBO” which can be seen in both the schematic and PCB editors.
Configuring properties for schematic components in Altium Designer
Configuring component properties in Altium Designer
When the designs are translated from EagleTM, the Unique ID values should match between schematic and PCB because the Eagle designs should be consistent. To control this, there is a very simple process to check the Unique ID values between the translated schematic to the translated PCB design:
- Open the ‘.PcbDoc’ file, and go to Project » Component Links
Configuring component links between a schematic and PCB
Any components appearing in the two left-hand panes do not have matching Unique IDs. The goal is to match a schematic component with a PCB component. This can be done manually by selecting a pair and using the > button to add it to the ‘Matched Components’ list in the pane on the right-hand side.
There is also an automated method, which will look at any combination of Reference Designator, Comment, and Footprint. Since the design was originally completed in EagleTM, the import process already used the reference designators to match between schematic and PCB.
The consistency will enable functions like cross-probing and Engineering Change Orders (ECOs) to operate much more accurately.
It is worth noting that there may not be a complete 1-to-1 match in the reference designator list. This may be due to mechanical type components added to the board but not the schematic, as fiducials, for example. Mounting holes added as components are another common mismatch. The reverse situation may also be true, where a component was added to the schematic to be included in the BOM, but has no physical representation in the PCB, such as a heat sink.
Altium Designer has several different component property options to define ECO behavior. Component properties in both the schematic and PCB editors include a list of available component types as shown below.
Configuring property options for ECOs in Altium Designer
You can read more about Altium Designer component types in the Component, Model, and Library Concepts article.
Setting elements, existing only in one domain, to Mechanical will remove it from the Component Links dialog. More importantly, it will also make the ECO process ignore them as a missing component. Otherwise, they would be removed during an ECO as it has no schematic counterpart.
There will always be at least a little bit of cleanup work to do. This is usually due to either incompatibilities between the two CAD systems’ data structures, or just differences in how certain features or object types were implemented.
In this section, we’ll address the common areas of the translated schematic that should be inspected. For this and subsequent cleanup sections, the assumption is that the user has at least a basic understanding of Altium Designer and how it’s used. To learn the basics of Altium Designer, please view the Getting Started with Altium Designer documentation.
For further information on editing multiple objects, please refer to the Editing Multiple Objects technical white paper.
In EagleTM, net connectivity is global. Usually there’s no need to place ports to connect nets crossing multiple schematic pages, but even so, they are usually placed.
Altium Designer can behave in the same way, but usually other structures are preferred. Hierarchical design, using ports and sheet entries to do a definitive and controlled net-connection between different schematic pages, is the common way to work. Within a schematic sheet, you can use wires and net labels. Between schematic sheets, nets in a flat design are typically connected using ports. 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. Ports and power ports are dedicated elements in Altium Designer. There’s no need to place them from a Library. The import process is capable of identifying and translating ports and power ports automatically. But of course, it’s a good idea to control this.
Two natural differences in the way to build up schematics in Eagle and Altium Designer should be checked and, if necessary, fixed: Bus constructions and shorts between wires. These connectivity problems become evident after running the project compile process (Project » Compile PCB Project) which runs the ERC (Electrical Rule Check). The Messages panel will report all errors and warnings, indicating any mismatches.
The message panel only opens if there are errors in your design, otherwise you’ll have to open it manually to view any Warnings (View » Workspace Panels » System » Messages).
Errors and Warnings in the imported Example
As Altium Designer does not support mixed bus structures (Harnesses would be used here) and the connectivity is sufficiently defined by Net Labels, the Net Labels defining the busses can be deleted without any replacement. In this way, the Buses will be seen as simple graphical lines. Below, the Status bus is connected using the label to establish a logical connection.
SHORTS BETWEEN WIRES
If an endpoint of a wire is placed on an electrical relevant element, a connection is established. In our example below, the net ‘EN’ shortcuts ‘STATUS0’ and the Bus. This can only be solved by redrawing ‘STATUS0’, or as shown, use a logical connection.
Wires shorted and wrong bus definition
PCB DESIGN CLEANUP
Although the translator does an excellent job of accurately converting the PCB data, incompatibilities between the two CAD systems could result in the need for further editing to the imported design.
When it comes to rule setup, EagleTM and Altium Designer are vastly different. While EagleTM uses a matrix-based basic rule set, Altium Designer enables you to define rules based on logic and set theory, not only regarding width or clearance but a wide range of additional setup possibilities in the electrical, mechanical and manufacturing area as well. So it’s a good Idea to adjust the design rules according to those new possibilities.
POLYGON (COPPER) POUR THERMALS
All PCB systems handle copper pour and thermal generation differently. Altium Designer takes an altogether different approach to thermal generation by managing these settings in the design rules (‘Polygon Connect Style rules’). In practice, this methodology allows a more dedicated thermal setup. The basic setup of the Eagle data is reflected in two rules which are generated automatically during the import process:
The first rule tells all vias to use “flood over” connectivity. This is achieved by setting the Scope to “IsVia” vs. “All” and the Constraints to “Direct Connect.
The second rule, having a lower priority, defines the remaining connections with thermal reliefs. In this rule, both the air gap as well as the conductor width can be defined.
For more information on design rule creation, please refer to Creating Design Rules within TechDocs.
ENGINEERING CHANGE ORDERS
Performing an ECO at this point should point out any remaining inconsistencies between the schematic and PCB. From the PCB, go to Design » Import Changes from
Manually matching net names confirmation
While there may be several changes required by the ECO process, one of the most important tasks is to rename the system- assigned net names. As discussed in the Schematic Import Process section, EagleTM and Altium Designer create system- assigned net names differently. It is generally recommended that you allow the ECO process to rename the EagleTM Capture names to Altium Designer names, as shown below.
System assigned net names in Altium Designer
Some other changes that may be requested by the ECO process can be controlled by selecting Project » Project Options. By doing this, Altium Designer will, by default, attempt to create, remove, and/or synchronize net classes, component classes, rooms, etc.
Configuring project options for an ECO in Altium Designer
It’s up to the user whether to accept these changes or not. The checkboxes in the ECO dialog allow the user to temporarily disable any particular change. Permanent changes to the types of modifications that are made during an ECO are controlled by going to:
Project -> Project Options menu, and then setting up the options in the ECO Generation tab.
There are a number of other situations that can cause the ECO process to show differences between the schematic and PCB. We don’t have the time to discuss them all here, but the user should be able to determine the sources of the differences by using the concepts we’ve provided. For more information, go to FindingDifferences and Synchronizing Designs within TechDocs.
Your ultimate goal is to receive a message after performing an update that indicates that no ECO will be generated, or that no differences are found (depending on how your Project Options are set).
No differences dialog
TRANSLATING YOUR LIBRARIES - EAGLESCHEMATIC SYMBOL LIBRARY
To translate an EagleTM library, you can simply import the .lbr file by following the steps below:
Select the File menu at the top of the screen, then select Import Wizard from the File menu.
The following dialog box will appear. Click Next to proceed.
Select the file type you wish to import Eagle Designs and Libraries Files. Click Next.
Click the ‘Next’ button to skip adding Eagle Designs Files. You can translate Design Files at the same time as Library Files (see above for details).
Click the ‘Add’ button to select the Eagle Library File(s) you wish to import. Click ‘Next’ to continue.
Other than the General Settings there is nothing more to adjust in the Reporting Options this time. Click ‘Next’ to continue.
The default project location for the import process is shown below. You can change the location if you wish. Click Next to continue.
If the translation process is successful, then the Wizard is complete. You can click to close it and start working on your translated Capture Libraries in Altium Designer. Click ‘Finish’ to complete the import process.
When the process is complete, the translated schematic library can then be opened from the Projects panel.
Projects Panel in Altium Designer
Most aspects of the schematic symbols and PCB footprints translate accurately. However, some minor editing may be necessary. For example, connecting one schematic pin to multiple Pads in the PCB is done differently in the both tools. While Eagle allows you to connect one pin with multiple different Pads in the pinning definition, Altium Designer enables you to use the same pad-number multiple times. That way, they are automatically connected correctly. And of course you’ll want to add 3D models to your footprints to enjoy the 3D capabilities of Altium Designer.
YOUR NEXT STEPS IN ALTIUM DESIGNER
Once all of your design files are successfully translated from EagleTM, it’s now time to dive deeper into the intricacies of the Unified Design Environment in Altium Designer. Below are several links to our documentation, video tutorials, and additional training resources, which will help you make the most of your experience in Altium Designer.
- Getting Started with Altium Designer - Explore a complete set of tutorials for creating your first schematic and board layout in Altium Designer.
- The Altium Designer Environment - Get a complete overview of the Unified Design Environment in Altium Designer.
- Library and Component Management - Learn how to easily manage your component libraries within your Altium Designer workspace.
That’s just a small sampling of the vast archive of Altium Designer documentation we have available. Explore more at Altium Designer technical documentation.
Our complete suite of videos includes several tutorials, feature overviews, and more to help get you acquainted with the Altium Designer environment. View all the available videos in the Altiumlive Video Library.
LIVE TRAINING EVENTS
Prefer a more hands-on approach to your learning? Register for one of our live events, including webinars, training courses, and seminars. View all the events on the Altium Events page.
NEED ADDITIONAL HELP?
Our support team is always here to assist you with any questions you might have. You can contact us directly through the Contact Us page.
WHY CHANGE & WHY NOW?
Are you falling short of meeting minimum design specifications, or missing release dates and product cost targets? Do you have the expertise to design the perfect board, but are unable to achieve your “feature elegance” targets due to the limitations of your design environment? Have you decided that it’s time to change your design software?
TOPICS IN THIS SOLUTION
With the rapidly increasing complexity of modern products, all with larger circuits in smaller packages, you can no longer accept the inability to meet your goals as normal and permissible. You require a complete PCB project solution that offers feature-rich products, state-of-the-art automation technology, intelligent analysis tools, and efficient time-tested collaboration across the entire ECAD-MCAD design process. Now is the time to take a closer look at Altium Designer.
OVERVIEW OF EAGLE™ PRODUCTS
Autodesk sells its PCB Design tool (Eagle) in three different stages of expansion:
WHY ALTIUM DESIGNER?
Your electronic designs demand the highest grade of efficiency and performance. When your productivity is measured against immovable deadlines, precise layouts, accurate documentation and exact fittings, you can’t afford to not invest in a complete PCB design platform. Altium Designer has everything you need to meet your design challenges and a proven track record of delivering innovative, differentiating features in predictable and reliable releases.
A cohesive environment for your design, data and release management process.
Altium Designer provides a cohesive PCB design environment that is easy to learn and use, following the Windows standard behavior. You have the features you need to make design decisions early, perform tasks efficiently and implement checks and balances throughout your design process. Altium Designer also interfaces seamlessly to third-party analysis, synthesis and 3D mechanical software.
With Altium Designer, you’re equipped with everything you need to solve even the most complex design challenges, including:
Supply Chain Integration
Always ensure you make intelligent part selections with real-time pricing and availability data from your most trusted and re- liable circuit board suppliers. Reduce the likelihood of costly and time-consuming design re-spins with complete visibility over supply chain data early in the design process.
Store all of your valuable design assets in a securely centralized location accessible by your entire design team. Ensure that your team is working with trusted design data with centralized library management tools and secure storage locations.
Flexible Release Management Tools
Control the consistency and reliability of your project with the ability to search and release accurate design data. Accelerate your design process by eliminating the need to reproduce data and documentation.
Seamless ECAD/MCAD Collaboration
Easily collaborate with your mechanical team in real-time with automatic data synchronization and tracking. Get your board manufactured right the first time with powerful Native3D™ visualizations and clearance checking with this PCB Simulation Software.
ALL WITHIN ONE, MODERN USER INTERFACE
All Altium Designer features are presented within one, modern user interface (UI). Whether you’re responsible for every aspect of the design process or delegated specific tasks, a consistent selection and editing paradigm allows you to quickly move between design tasks. The context sensitive UI changes when you switch from one aspect of the process or document to another, providing you with the most relevant and intuitive selections. If you focus solely on one element of the design process, the UI can be configured to match your preferences. The consistent look & feel allows you to quickly become proficient as you take on additional design tasks.
Unified UI, show schematic/layout side-by-side
LIBRARY AND COMPONENT MANAGEMENT IN EAGLE
Eagle offers a file-based library which incorporates common file access limitations to share library content with other team members. There’s also a feature that allows you to add design links to components to maintain the synchronization across your schematic and PCB layouts. This is something note when considering whether Eagle vs. Altium Designer PCB Software best meets your needs.
LIBRARY AND COMPONENT MANAGEMENT IN ALTIUM DESIGNER
Altium is the leader in providing a complete solution for the PCB design, development and production process. One of the fundamental aspects of this process includes a close connection to supply chain and real-time component management. In Altium Designer, there are different library concepts available. Starting with easy file-based structures to database-driven libraries supporting collaboration as well as managed libraries which give you the means of maintaining lifecycles and revisions. Whichever option you choose the setup and use is fast and easy while maintaining a light footprint.
Real-Time BOM Management in Altium Designer - ActiveBOM®
ActiveBOM® offers a live presentation of the design from the outset, providing early and ongoing critical supply chain information, such as availability and pricing. Altium Designer ActiveBOM facilitates real-time cost estimation and tracking for your board design, by bringing to the table a system that effectively and efficiently aides you in managing costs and availability of items used in your printed circuit board design. It allows you to define target pricing at the individual item level. You can then track how actual costing fares against these estimates, and gives you a timely flag if any cost blow-outs are on the near horizon. In addition, you can quickly assess item availability, complete with notification if there is a risk in the supply of a chosen part (i.e a part going into End-of-Life state). ActiveBOM also allows specifying pin-compatible backup part choices directly in the BOM referred to as alternative part choice. Having pin-compatible backup part choices nearly eliminates supply chain issue risks for manufacturing. In turn, you can design while taking into account potential manufacturing blowouts, reducing time to market and minimizing unexpected costs and design changes.
ActiveBOM - Real-Time Cost Estimation & Part Availability
EAGLE SCHEMATIC CAPTURE
Eagle offers a nice schematic entry that provides the most commonly needed features. However, there are some obvious limitations when it comes to bottom-up development of hierarchical designs, controlled reuse and snapping outside the standard grid. With the user-interface being quite different from the Windows world, there can be a learning curve that could result in one or two gray hairs.
ALTIUM DESIGNER SCHEMATIC CAPTURE
Altium Designer schematic capture technology has long been recognized as a technology differentiator. Engineers and designers will find that Altium Designer schematic features are easy to learn and quickly improve productivity on all designs ranging between relatively simple single-sheet schematics to complex multi-sheet hierarchical projects with complex schematic symbol use. Here’s why:
Modern and powerful Unified Schematic Editor
- Starting a schematic is fast and easy with intuitive dialogs, e.g., editing workspace and establishing sheet design, parameters, preferences and associated documents. Immediately manage versions.
- Easily set component classes, net classes, and placement rooms in an intuitive environment that boosts productivity.
- Quickly select and place qualified components from integrated libraries with real-time links to component suppliers.
- Leverage powerful ECO feature to transfer a captured design to a new PCB, make changes to an existing design on either the schematic or PCB, synchronize the schematic and board, and compare and resolve differences.
- Verify your circuits using the built-in XSPICE/SPICE3F5 (PSpice® model compatible) circuit simulator without leaving the environment.
RULES AND CONSTRAINTS IN EAGLE
In Eagle, you’ll find a basic, matrix-driven way to configure minimum clearances, file formats, and width definitions for elements and net classes. More complex rulesets that take different Layers or specific areas on the PCB into account cannot be defined. This also includes length definition sets for partial nets, which are needed in high-speed designs like DDR3 or 4 technology, or differential pairs with serial terminations.
RULES AND CONSTRAINTS IN ALTIUM DESIGNER
True to its cohesive and easy-to-use nature, Altium Designer provides a streamlined PCB Rules and Constraints Editor, with more control over the entire design process:
Constraint Driven PCB Design with Design Rule Checking
- Easily browse, create, prioritize, define the scope, edit, duplicate and delete rules all in one editor.
- Evaluate your rules in a table-based summary that provides straightforward review.
- Define multiple rules of the same type, but each targeting different objects.
- Decide exactly what a rule’s precedence will be and how it will be applied to target objects through a query.
- Write your own, more complex queries using Advanced Query options.
- Create new rules in a step-by-step manner with the New Rule Wizard guiding you along the way.
PLACEMENT AND ROUTING IN EAGLE
Being able to place components solely within the boundaries of a PCB limits the developer when cleaning up the mess of components caused by the automatic, uncontrollable and disorganized schematic-to-PCB synchronization. The idea of sorting and placing components according to their destination task and possibly routing those modules is completely impossible in this way. Even more annoying is making adjustments when most of the routing work has already been done, as routing the last set of tracks often requires pushing other tracks away. An alternative to deleting and redrawing those tracks manually should exist to facilitate the routing process for designers.
PLACEMENT AND ROUTING IN ALTIUM DESIGNER
It’s crucial to have an organized and efficient placement of components on your PCB. Altium Designer offers enhanced capabilities to ensure proper component placement and create the most efficient board layout possible:
Routing in Altium Designer
- Dynamically place and drag components that push, avoid, and snap-to alignment with other components on your board layout.
- Easily align multiple components to keep your board layout organized and tidy.
- Mask or filter objects in the workspace to gain more visibility over your board.
- Optimize your routing layers with the Layer Stack Manager giving you full control over all layers.
FAST AND HIGH-QUALITY ROUTING IN ALTIUM DESIGNER - ACTIVEROUTE®
ActiveRoute, included in Altium Designer, brings a new approach to interactive routing - select the connections and ActiveRoute them to produce high-quality routes, in a fraction of the time it would take to manually route them. Rather than allowing an autorouter to do its best at routing the entire board, ActiveRoute acknowledges the reality that board design is a highly interactive process, where the best results are produced by skilled designers using powerful tools under their control. Altium Designer enables this by giving you easy, intuitive control over the selection of the connections or routes of interest.
Unlike other interactive routing technologies, ActiveRoute works on multiple layers simultaneously while adhering to your design constraints so you don’t have to worry about breaking any rules. It also has strong support for modern design techniques, including differential pairs and room-based width requirements. ActiveRoute lets you break out and route large, fine-pitch BGAs by instructing it where to route them (i.e. select layers, draw a guide path), and letting it do the heavy lifting for you.
Complementing ActiveRoute, the Glossing engine carefully analyzes selected routes, neatening and shortening them. The Glossing engine also delivers a Retrace Selected command, which can be used to update the selected routes to the current routing rule settings - this enables you to fatten up that existing power routing, or update that differential pair to new width and gap settings. By routing on multiple layers simultaneously, routing is faster, traces are evenly distributed, and the ability to complete the routes increases significantly. The result: a beautiful, expert, manual-like, glossed routing, without the hours of manual work.
ActiveRoute With Length Tuning - Before and After (25 Seconds later!
OTHER DIFFERENTIATING PLACEMENT AND ROUTING FEATURES IN ALTIUM DESIGNER
- Eliminate the stress of your manual routing process with powerful interactive routing modes and an intelligent routing assistant.
- Easily save, share, and reuse your most trusted design assets with smart, copy-and-paste managed schematic sheets and component library templates.
- Gain even more control over your clearance checking with enhanced test point clearance checks between test points, through-hole pads, and inter-test point spacing.
- Get even more precise with your solder mask expansions with user-definable expansion options from hole edge or pad edge.
- Intelligently route your rigid-flex board layout in Native 3D, then visualize your work of engineering art.
Altium is continually adding more powerful and differentiating placement and routing features to Altium Designer. These features will increase your productivity, streamline your core PCB design tasks, and reduce your time to market.
xSignals - Automated High-Speed Signals for High-Speed Topologies
See the Altium Designer product website for examples of the many benefits you can reap and the new features you can explore: https://www.altium.com/altium-designer/whats-new.
DESIGN COLLABORATION IN EAGLE
Mechanical and 3D are not really part of the Eagle environment. Although first steps have been taken - IDF 3D export and scripts are available for generating 3D data - Eagle itself only provides a 2D PCB editor requiring export to Fusion 360™ or other MCAD tools for clearance checking making it slow and iterative to resolve placement issues.
DESIGN COLLABORATION IN ALTIUM DESIGNER
Altium Designer was the first PCB design product to provide true ECAD/MCAD collaboration with 3D editing features powered by the Native3D™ PCB editor engine to visualize, compare, merge, track, and comment on design changes. Electrical and mechanical design data integrates seamlessly into your workflow with real-time visibility into incremental changes. This allows the electrical and mechanical engineering work to be done simultaneously and in parallel.
You can visualize exactly how your board will fit its mechanical enclosure and fix collision errors in seconds. You can perform real-time clearance checking for components and mechanical enclosures, and generate folded STEP models.
3D Mechanical Collision Detection & Clearance Checking in Real-Time
RIGID-FLEX 3D PCB MODELS
A significant differentiator, Altium Designer supports 3D rigid-flex design. With this feature, you can easily define material selections and intelligently route your rigid-flex board layout, then dynamically visualize your engineering work of art in 3D to make sure that the folding/folded board does not create violations in real time.
INTERCONNECTED MULTI-BOARD ASSEMBLY
With circuit boards not existing in isolation and often assembled together with other boards, which are then housed inside an enclosure, Altium Designer now supports creating and managing multi-board assemblies. You can define the logical (schematics) structure of the system in a multi-board schematic, with each logical block in the multi-board schematic referring to a physical (PCB) design. Then the physical multi-board design is created by transferring the system design into a multi-board assembly design. This enables designers to verify at the system level how their “child” PCBs are electrically and physically connected while maintaining the integrity of their pin and net connectivity.
Altium Designer gives you the design space where you can plug together multiple boards, and the tools to manage the whole system connections, resolve conflicts, and update system-child projects. And with the state-of-the-art 3D multi-board assembly editor, you can have the separate boards be rotated, aligned and plugged into each other. It also allows other parts, including other boards, assemblies, or STEP format MCAD models, to be imported and positioned in the assembly.
Altium Designer brings you system-level design capabilities to the electronic product development process so you can verify if nets have been assigned correctly, connectors are oriented correctly, plug-in boards fit together, and whether all the connected boards fit into the enclosure. This helps minimize any costly late development stage mistakes or time to market delays.
Multi-board Assembly Management
STREAMLINE ASSEMBLY AND FABRICATION IN ALTIUM DESIGNER
A powerful automated PCB design documentation tool is available directly within Altium Designer: Draftsman®. It automates the creation of tables, PCB design views, layer stack legend, and other details. The drawing document is linked to the source PCB document so they are always accurate and in sync.
Multi-board Assembly Management
FOR A FULL EVALUATION
Obtain a 15-day full featured evaluation license at https://www.altium.com/free-trial.
EAGLE and Fusion 360 are trademarks of Autodesk Inc. and PSpice is a registered trademark of Cadence Design Systems Inc. and Altium claims no rights there within.