Keeping the Schematics & PCB Synchronized

Altium Training

Altium Essentials: Transfer to PCB

This content is part of the official Altium Professional Training Program. For full courses, materials and certification, visit Altium Training.

At a Glance

This article explains how Altium Designer keeps schematics and PCB layouts synchronized, from the first transfer of a captured design to ongoing updates made on either side. It walks through how the comparator detects differences, how Engineering Change Orders are created to resolve them, and the two main synchronization approaches, bi-directional and single-direction updates. It also highlights what kinds of data can be synchronized, how comparator and ECO options affect the process, and how classes and design rules can be carried across as part of synchronization. If you want a clearer understanding of how to keep your design aligned and reduce manual rework, this guide will help you work with more confidence, keep reading.

- Learn the difference between bi-directional comparison and direct update workflows, and when each approach is used.
- Understand what Altium Designer can synchronize between schematic and PCB, including components, connectivity, classes, and certain design rules.
- See how project options like Comparator and ECO Generation settings influence the synchronization process and the changes that can be applied.
Go Deeper with AI:

The most common schematic-to-PCB design task is keeping the schematic and PCB matched, or synchronized.

Whether you are transferring a captured design to a new PCB for the first time, or making changes to an existing design on either the schematic or PCB side, you need some way to keep the two sides in-sync. Altium Designer includes powerful design synchronization capabilities that simplify the task of keeping the design synchronized, allowing the designer to keep their focus on the creative aspects of the design process.

The synchronization process detects and resolves the schematic and PCB differences. The synchronization process detects and resolves the schematic and PCB differences.

Design synchronization is performed directly between the schematic and PCB editors; there is no intermediate, netlist-like document used. The software uses a comparator engine to compare all aspects of the design, detailing the output as a list of differences. The designer decides which side should change to resolve the differences, and a set of Engineering Change Orders (ECOs) is created. When these are applied, the two sides of the design are back in sync.

Approaches to Synchronizing

There are two approaches to performing a synchronization:

  • Single-direction synchronization – the more common approach, used to push all changes from the schematic to the PCB, or from the PCB back to the schematic. This done using the Design » Update PCB or the Design » Update Schematic commands from the respective editors (Synchronization Process). Refer to the Performing a Direct Update section to learn more about this approach.

  • Bi-directional synchronization – where differences can be updated in both directions simultaneously using the Project » Show Differences command, as shown in the image above. Bi-directional synchronization is typically only used in the specific situation where the design is being modified in both the schematic and PCB spaces at the same time. Refer to the Detecting the Difference Between Designs section to learn more about this approach.

Before transferring the schematic information to the new PCB, it is essential that all the related libraries for both schematic symbols and PCB footprints are available.

What Can be Synchronized?

The synchronization process ensures that the component and connective data on the schematic, matches the component and connective data on the PCB. As well as the component and connective data, the synchronization process also ensures that other design constraints; such as net classes, component classes and design rules, are also in sync.

Configuring the Comparator Options

The first stage of the synchronization process is to compare the schematic to the PCB. Exactly what schematic and PCB data gets compared is configured in the Comparator tab of the Options for PCB Project dialog. Select Project » Project Options to open the dialog.

The comparator engine obeys the settings defined in the Comparator tab of the Options for PCB Project dialog.
The comparator engine obeys the settings defined in the Comparator tab of the Options for PCB Project dialog.

Learn more about the Comparator tab of the Options for PCB Project dialog.

Synchronizing Net and Component Classes

As well as component and connective data, you can also generate and synchronize classes when you perform a Design » Update PCB. Classes are a logical collection of a particular type of design object. For example, a group of related components could be grouped into their own Component Class, which could then be used as the basis for creating a targeted rule. Use this tab to configure the generation of both automatically generated classes and user-defined classes, when the source schematic documents are synchronized with the PCB design document.

The Class Generation tab of the Options for PCB Project dialog.The Class Generation tab of the Options for PCB Project dialog.

Learn more about setting up the Class Generation tab.

Learn more about the generation and synchronization of classes from the schematic.

Synchronizing Design Rules

For a project using design rules (rather than the Constraint Manager), rules can be defined on the schematic by adding it as a special type of parameter. For schematic objects that include parameters, such as components, the rule is added in the Parameters section of the Properties panel. Otherwise, the rule is defined by placing a Directive, such as a Parameter Set or Differential Pair, so that it touches the object the rule is to apply to.

In the image below, a width constraint design rule that targets specific nets is being defined on the schematic, by defining the rule within a Parameter Set object. Rather than placing a Parameter Set object on each wire that needs a rule, a Blanket directive has been placed so that it covers both the net identifiers D- and D+, and then the Parameter Set object placed so that it touches the Blanket. The software knows that the requirements defined in the Parameter Set must be applied to all nets detected under the Blanket. As well as the width constraint, the Parameter Set also specifies that all nets detected under the Blanket are to be made members of the USB_data Net Class. This results in a single Width Constraint design rule being created in the PCB editor, scoped to target the USB_data Net Class.

The Parameter Set is used to define a net class and a design rule, to the nets under the schematic blanket object. Note that the required measurement units are configured at the bottom of the Edit PCB Rule dialog.
The Parameter Set is used to define a net class and a design rule, to the nets under the schematic blanket object. Note that the required measurement units are configured at the bottom of the Edit PCB Rule dialog.

Learn more about defining a design rule in the schematic.

Learn more about configuring differential pairs on the schematic. 

Configuring the ECO Generation Options

The Options for Project dialog also includes an ECO Generation tab. This tab defines which design modifications can have ECOs created. Typically these are all enabled, with the options in the Comparator tab of the dialog being used to configure which design changes are to be synchronized between the schematic and the PCB.

The ECO Generation tab defines which types of modifications can have ECOs created.
The ECO Generation tab defines which types of modifications can have ECOs created.

Performing a Direct Update

Since the designer usually knows which way they want to apply the updates and those updates are all in the same direction, the most common approach to synchronizing is to perform a direct update. To do this you choose the Update command from the Design menu, from either the schematic editor or the PCB editor. Your choice of editor from which you run the command indicates the direction you want the changes to be made - from this editor, to that editor. For example, you would choose Design » Update in the schematic editor to push all changes from the schematic to the PCB.

The active PCB design document can also be with any changes that have been made to the source schematic documents by choosing the Design » Import Changes from <ProjectName> command, from the main menus of the PCB editor. Using this approach, the Differences between dialog is skipped and you jump straight to the Engineering Change Order dialog.

If all of the updates are going to be applied in the same direction, use the Design » Update command. If all of the updates are going to be applied in the same direction, use the Design » Update command. 

If the PCB document is currently synchronized with the source documents, a dialog will appear stating that no differences were detected. Conversely, when updating schematics, it is also possible that some, or none of the detected differences, can be resolved by automatically generated ECOs. In this case, you will be given the option to view these differences, through the Differences between dialog. While a modification may not be possible in the direction of the schematics, it may be that you need to update the PCB (perhaps by removing an object or entity). After sifting through the differences, if you are able to resolve some, or all of them, you can generate an ECO. If there remain differences that can't be resolved through the dialog, you will need to return to the design to resolve the issues, before running a comparison again.

Resolving Differences - Applying the ECOs

Each difference is resolved by applying an Engineering Change Order (ECO). The modifications required in the ECO are listed in the Engineering Change Order dialog with one modification per line, each with its own Enable checkbox. The dialog has two main sections – Modifications that details each action, the objects it applies to, and the documented impacted by that change; and Status, which details if the action could be and has been applied.

Each design change presents as an ECO, enable those that are required.
Each design change presents as an ECO, enable those that are required.

Comparator-related messages will be displayed in the Messages panel.

Detecting the Difference Between Designs

Altium Designer can compare any two designs and detail the differences between them. The Choose Documents to Compare dialog is used to select what two documents/document-sets to compare, for example the schematic project against the PCB. You can also use this dialog to compare any document to any document by ticking the Advanced Mode option.

Support for detecting differences includes:

  • Show Differences – a logical comparison of one design against another, for example a schematic design against the PCB, or a netlist against the PCB.

  • Show Physical Differences – used to perform a physical (graphical) comparison of one schematic or PCB document, against another. 

Both the Project » Show Differences and Project » Show Physical Differences commands open Choose Documents to Compare dialog, as shown belowi.

Use the Show Physical Differences command to detect the physical differences that exist between two versions of a schematic or PCB document, and present these differences graphically when viewing the two documents side-by-side in the design space. The Show Physical Differences feature offers purely visual comparison – the command does not lead to the generation of ECOs. It is intended for comparison of two versions of the same document, with the Differences panel appearing to explore the differences.

Choose Documents to Compare dialog

Comparing the PCB (Kame_MB.PcbDoc) to the schematic project (Kame_MB.PrjPCB).

Choose Documents to Compare dialog

Using the Advanced mode to compare one version of the board (Kame_MB.PcbDoc) against another version (Copy of Kame_MB.PcbDoc).

 

Exploring Design Differences

The design synchronization feature is able to detect and resolve differences in both directions; that is, from the schematic to the PCB, or from the PCB back to the schematic. When the comparator engine compares the schematic project to the PCB, a complete list of differences is created - at this stage there is no assumption on which side must be changed to bring them back into sync.

The software is capable of resolving these differences by applying changes to both sides, at the same time. For example, imagine the scenario where the electronics designer has changed the value of a capacitor, while the PCB designer has changed the footprint of that same capacitor. These two differences can be resolved in a single update process, by applying the comment change as a schematic-to-PCB update, and the footprint change as a PCB-to-schematic update (Synchronization Process).

The list of differences can be seen in the Differences between dialog.

There are two approaches to detecting and resolving differences: either assign the update direction for each change, or, apply all updates in the same direction. Continue reading to learn how to perform a bi-directional synchronization. If you do not need to apply updates in both directions at the same time, then you do not need to go through the process of choosing the documents to compare and configuring the update direction for resolving the differences. In this case, you can go straight to the Performing a Direct Update section of this page.

The Differences Panel

The Differences panel is used to display the logical or physical differences found by the software's built-in Differences Comparator when comparing design documents (for example, when comparing the source document hierarchy (schematics) for a project against the PCB design document). The panel allows you to interactively explore the differences before the decision to create an Engineering Change Order (ECO) that will be used to synchronize the project documents.

Click on an entry in the results to cross probe to that object in the design.

The Differences panel displays a hierarchical view of document differences.
The Differences panel displays a hierarchical view of document differences.

Understanding the Linking Between the Schematic and the PCB

Rather than relying on the designators to link the schematic and PCB components, Altium Designer uses unique identifiers.

Component Matching via Unique Identifiers

Each schematic component links to its PCB component through a Unique Identifier (UID). The UID is automatically assigned when the schematic component is placed on the sheet. When component information is transferred for the first time between source schematic documents and the blank PCB using the Design » Update PCB command, each PCB component is automatically assigned the UID from the matching schematic component.

While this scheme would be adequate for a simple design, it is not capable of supporting a multi-channel design. In a multi-channel design, the same schematic component is repeated in each physical channel, which would mean the repeated PCB components would have the same UID. To cater for this, the UID for the PCB component is actually created by combining the UID of the parent Sheet Symbol with the UID of the schematic component. The syntax of the PCB UID changes slightly, depending on how the multi-channel design has been created.

For a multi-channel design created by placing multiple Sheet Symbols that all reference the same schematic sheet, each Sheet Symbol can provide a unique ID so the PCB UID has the format:

\SheetSymbolUID\SchComponentUID

For a multi-channel design created using the Repeat keyword, there is only 1 Sheet Symbol UID available, so the PCB UID also includes the ChannelIndex value, in the format:

\ChannelIndex+SheetSymbolUID\SchComponentUID

Note that the UIDs are not displayed in panels and dialogs.

When the Components are not Linked

The advantage of using a UID to match the schematic and PCB components is that it allows the designators to become unsynchronized (perhaps by performing a PCB re-annotate a number of times), without any risk of the schematic and PCB becoming unsynchronized.

During design synchronization, if there is a component present on the schematic or the PCB that does not have a matching component (same UID) present in the other editor, the following will occur:

  • If the extra component is only present in the source editor, an ECO is created to add the component to the target editor.

  • If the extra component is only present in the target editor, an ECO is created to remove the extra component.

  • When there are unmatched components present in both editors the software needs instruction on how to deal with them, so the Failed to Match Unique Identifiers dialog opens.

The Failed to Match Unique Identifiers dialog.The Failed to Match Unique Identifiers dialog.

Manually Linking Components

The status of the component links between schematic components and their corresponding PCB component footprints can be checked and managed at any time, in the Edit Component Links dialog (PCB editor, Projects » Component Links command). Components that are unmatched are presented in the two Un-Matched Components columns on the left, components that share a matching UID are presented in the Matched Components region on the right of the dialog.

The reason that manual linking of components is only carried out from within the PCB document is that only the PCB component footprints ever have their component unique ID information updated – the schematic components are the source so are never updated. If any updates are performed, then the PCB must be saved.

The Edit Component Links dialog is used to detect and resolve UID mismatches, it must be run from the PCB editor.
The Edit Component Links dialog is used to detect and resolve UID mismatches, it must be run from the PCB editor.

Matching the Nets and Classes

Both nets and classes have a parent (the net or class), and children (the members of that net or class). Matching these requires a different approach than the UID mechanism used for component linking, to support changes to: the parent; the children; or both the parent and its children. For example, something as simple as changing the name of a net on the schematic should not require that net and all its children pins be removed from the PCB, then the newly named net be added, and finally all the children pins be added to that new net.  

To support this, the software includes separate matching algorithms to match nets and classes by their members, and also by their name. The matching process is configured in the Object Matching Criteria section of the Comparator tab of the Options for Project dialog.

The default settings is to match members first, then by Object Type name.
The default settings is to match members first, then by Object Type name.

Matching for these types of objects is handled in the following way:

  1. During design synchronization, the default behavior is to first attempt to match by members (configured in the Use Name Matching column), in accordance with the Min Match % and Min Match Member settings.

  2. If member matching fails, the software will then attempt to match by name (if the Use Name Matching option is not set to Never).

  3. If either of these matching processes succeeds, you will proceed to the Engineering Change Order dialog.

  4. If both matching techniques fail (or the Use Name Matching option is set to Never), the Match Manually dialog will open ().

  5. Clicking No in the Match Manually dialog will skip the user-matching process and jump straight to the Engineering Change Order dialog. Since you have not attempted to match any unmatched objects, the software assumes that the reference and target objects are unrelated, so ECOs will be generated that remove the Unmatched Reference Objects from the board, and add the Unmatched Target Objects as new objects.

  6. If you click Yes in the dialog to match manually, the Match dialog will open, as shown below (the dialog caption changes to suit the unmatched object type).

The Match dialog is used to manually match objects that you know to be matched. Leave the right side empty and click Continue if you are unsure.The Match dialog is used to manually match objects that you know to be matched. Leave the right side empty and click Continue if you are unsure.

Matching the Design Rules

Design rules that are defined on the schematic are linked to the matching rule on the PCB. UIDs are used to link the schematic design rule to the PCB design rule, allowing you to update the rule on the schematic and flow those changes to the PCB, and to rename the rule in the PCB editor. The UID is automatically assigned in the schematic editor, and transferred to the PCB during design design synchronization.

Design rules use a UID to match the schematic design rule definition to the PCB design rule.Design rules use a UID to match the schematic design rule definition to the PCB design rule.

  • Typically, you will not need to manually manage the matching of rules, unless you have manually edited the UID in the PCB Rules and Constraints dialog in the PCB editor.

  • If the UIDs do not match, the software will add a new rule to the PCB for any schematic rule that does not have a matching PCB rule, and remove any PCB design rule that does not have a matching schematic design rule.

  • If you do not want to remove rules defined in the PCB editor that have not been defined in the schematic, enable the Ignore Rules Defined in the PCB Only option in the Comparator tab of the Options for Project dialog ().

You can freely update components in either editor and synchronize those changes to the other editor. Changes made to nets, classes, and rules can only be updated from the schematic to the PCB. 

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Contents
Feature Availability

The features available to you depend on which Altium solution you have – Altium Develop, Altium Agile Teams, Altium Agile Enterprise, or Altium Designer (on active term).

If you don’t see a documented feature in your actual software, contact Altium Sales to find out more.

Legacy Documentation

Altium Designer documentation is no longer versioned. If you need to access documentation for older versions of Altium Designer, visit the Legacy Documentation section of the Other Installers page.

Contents