Keeping the Schematics & PCB Synchronized in Altium NEXUS

Parent page: Working Between the Schematic and the Board

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 NEXUS 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.

Design synchronization is performed directly between the schematic and PCB editors. 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. These are then applied, bringing the two sides of the design back in sync.

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

Dialog page: Options for PCB Project, Comparator tab

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 Project dialog.

The main region of the dialog includes a large list of Comparison Types, such as Different Designators and Changed Net Name, which are grouped in 5 categories. The Mode column on the right includes a dropdown for each, where you select the mode of comparison, such as Find Differences or Ignore Differences. Text-type comparisons have a third option, to allow the comparison to be case-insensitive.

The default for a new project is to Find Differences for every comparison type, set the options as required for your project.

Across the bottom of the dialog there are options for setting the Object Matching Criteria. Matching is a sophisticated, multi-pass process that does not rely on simple exact string matching. To learn more, refer to the Matching the Nets and Classes section. 

Note the Ignore Rules Defined in the PCB Only option down the bottom of the dialog, enable this to exclude the rules you have defined in the PCB, from the comparison process.

Synchronizing Net and Component Classes

Dialog page: Options for PCB Project, Class Generation tab

As well as component and connective data, you can also generate and synchronize classes and design rules when you perform a Design » Update PCB.

Synchronizing Design Rules

Design rules can be defined in the schematic, using a Parameter Set object. When a Parameter Set object is selected, the Properties panel or modal dialog includes a Rules region. Click the Add drop-down to add a design rule. The rule will be applied to the net / bus / harness / objects under the blanket, which the Parameter Set object is touching.

In the image below, a width constraint design rule is being applied to the USB_data net class (the net class is also defined as part of this Parameter Set, in the Classes region of the Parameters drop-down).

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.

Adding a Design Rule in the schematic

1. Attach a Parameter Set to the net / bus / harness / blanket (add a Net Class definition in the Parameter Set, if required).
2. Add a Rule definition in the the Parameter Set. This will open the Choose Design Rule Type dialog, as shown above.
3. Select the required Rule Type.
4. Click the OK button to open the Edit PCB Rule dialog.
5. Configure the PCB rule requirements as required. Note that the measurement units required for this PCB rule are selected at the bottom of the dialog.

In both the image above and the image below, the design rule is defined in a Parameter Set object that is attached to a blanket. By including a Class definition in the Parameter Set object, a PCB net class will also be created, and because the class definition is present, the PCB rule will be scoped InNetClass('<PCB_NetClassName >'). 

In the image below you will notice that the Parameter Set object is displayed as a Differential Pair directive. This is a special type of Parameter Set object, placed using the Place » Directives » Differential Pair command.  

The Differential Pair directive is used to define a net class and a design rule, which is then applied to targeted diff pairs.

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.

Finding 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.

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.

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 list of differences can be seen in the Differences between dialog. To open the Difference between dialog and see a list of differences:

• Run the Project » Show Differences command to open the Choose Documents to Compare dialog, as shown in the image below. The Choose Documents to Compare dialog is used to select what two documents/document-sets you will be comparing, typically it is 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. For example, you might be comparing a netlist to a PCB, or a PCB to a PCB.

Select the PCB to compare the schematic project against.

• Select the PCB in the main part of the dialog, and click OK to open the Difference between dialog, as shown below.

The Differences between dialog will open. The next step is to assign an update direction to each difference:

• For an individual difference, click in the Update column to display a direction selector, as shown in the image below.
• For multiple differences of the same kind, right-click on a heading, such as Different Footprints, and select the required Update Same Kind command.
• For all differences, right-click anywhere in the dialog and select the required Update All command.

For each difference, the Update direction must be set for an ECO to be created to resolve that difference.

Click the Explore Differences button to access the Differences panel and explore the differences as described in the Exploring Design Changes with the Differences Panel section below.

Once the Update direction has been assigned, click the Create Engineering Change Order button to open the Engineering Change Order dialog, which is described in the Resolving Differences - Applying the ECOs section below.

Exploring Design Changes with the Differences Panel

The Differences panel displays a hierarchical view of document differences.

Summary

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.

Panel Access

To open the Differences panel:

• Choose View » Panels » Differences from the main menus.
• Click the Panels button on the bottom right-hand side of the design workspace, then click Differences.

Displaying Differences

How the Differences panel is applied depends on whether the goal is to:

• Analyze the integrity of the complete project in terms of its content and structure by detecting logical differences within the project hierarchy.
• Compare two versions of the same Schematic or PCB document by detecting their graphical (physical) differences.

Displaying Logical Differences

Comparison of project documents for logical differences is done in the Choose Documents To Compare dialog, activated by right-clicking on a project (or project document) in the Projects panel then selecting Show Differences from the associated context menu.

Right-click on a project name then select Show Differences to open the Choose Documents To Compare dialog.

Typically, the PCB document would be compared against the source document hierarchy for the parent project to detect logical differences between the schematic design content and the PCB design content.

After clicking OK, if any differences exist between the nominated documents, the Differences between dialog will open. Information in the Differences panel will only appear after clicking the Explore Differences button in the Differences between dialog.

The Differences panel will display only the differences that are listed in the Differences between dialog. These, in turn, are determined by the selections made in the Comparator tab of the Project Options dialog (Project » Options). This tab lists all of the comparison types, such as differences associated with Components, Nets and Parameters. Setting the Mode for each comparison category between Find Differences or Ignore Differences will determine if the Differences Comparator passes its results into the Differences between dialog.

Set up how the differences are detected and reported in the Project Options dialog.

The Differences panel displays the differences found between source documents in a tree-like structure, where the top-level folder displays the total number of differences detected. Sub-folders are then created for each specific comparison type that appears in the Differences between dialog. Each sub-folder lists the specific differences that have been found, which, in turn, are broken down further into objects on the documents that are responsible for creating those differences.

If the associated document is open (or open and hidden), clicking on an object entry in the panel will cross-probe to the object on the document.

The visual display of the object uses the zoom and dim effect where the object is highlighted by dimming all other objects. The contrast of the dimming can be varied with the Dimming slider found in the Highlight Methods region of the System - Navigation page of the Preferences dialog.

Displaying Physical Differences

The graphical (physical) comparison of two versions of the same schematic or PCB document is carried out basically in the same way as the logical comparison outlined above, but also makes use of the Advanced Mode in the Choose Documents To Compare dialog.

Perform a document physical comparison using the Show Differences command (Projects panel right-click menu) to open the Choose Documents To Compare dialog then check the Advanced Mode box. With all project files now shown in the dialog, select the two variations of a document for comparison.

Selecting documents for physical comparison from the Choose Documents To Compare dialog in Advanced Mode.

Clicking OK will proceed with the graphical comparison and open the Differences between dialog as outlined previously. Click Explore Differences to open the interactive differences list in the Differences panel.

The panel displays the differences found between the documents in a tree-like structure. The top-level folder displays the total number of differences detected. Entries are created for each type of difference, which, in turn, contains the specific references and the object (port, part, etc.,) involved for each.

Selecting the object entry for a detected difference will highlight and zoom to the object in the editor workspace.

Notes

• If an object in the panel resides on a document that is currently hidden, the document will be opened automatically and made the active document in the design editor window when you click the associated entry.
• The filtering applied when cross-probing from the Differences panel is temporary. As such, you are not prevented from selecting or editing design objects that fall outside the scope of the filter.
• The information in the Differences panel will be cleared when performing a new document comparison or compiling the parent project.

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, you can choose to skip the difference detection and direction assignment process that has just been described.

Rather than selecting the Show Differences command from the Project menu, 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 Differences between dialog will be skipped and you will 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. 

Resolving Differences - Applying the ECOs

Dialog page: Engineering Change Order

Each difference is resolved by applying an Engineering Change Order (ECO). The ECOs are listed in the Engineering Change Order dialog with one ECO per line, each with its own Enable checkbox.

When using the Engineering Change Order dialog:

• The dialog opens with all changes enabled, disable any changes you wish to hold off for now. The dialog supports multi-select - use the right-click context menu to toggle the enable state of selected ECOs.
• Use the right-click Cross Probe command to examine the objects affected by that ECO.
• Use the Validate Changes button to check that the changes can be performed. ECOs typically fail because an object is not available - for example, the specified PCB footprint does not exist in the Available File-based Libraries, or the specified pad does not exist on the footprint.
• An ECO can also fail because an object that is needed by a certain ECO was not present, but was added during the processing of the current ECOs. In this situation, run the Update command again to complete that ECO.

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

Understanding the Linking Between the Schematic and the PCB

Component Matching via Unique Identifiers

Each schematic component links to its PCB component through a Unique Identifier (UID). The UID is assigned when the schematic component is placed on the sheet, and this value is transferred to the PCB component when the design is transferred to the PCB editor.

This scheme would be adequate for a simple design, but 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 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, then 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

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 unsynchronizable.

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 to add the component to the target editor will be generated.
• If the extra component is only present in the target editor, an ECO to remove the extra component will be generated.
• 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 dialog buttons have the following options:

• Automatically Create Component Links - click this button if you know that the unmatched components already have matching designators. Using the component designators, the software will assign matching UIDs to these extra components. For components that can be matched by designator, any other property differences (such as unmatched parameters), will result in ECOs being generated. If there are components that cannot be matched by designator, ECOs to add/remove these will be generated (extra components present in the source editor to be added, extra components in the target editor to be removed).
• Manual Component Links - click this button if you know there are components that match, but do not know the status of their designators. The Edit Component Links dialog will open (described below), where you can manually select each source and target component and transfer them to the matched components list, assigning them matching UIDs. ECOs will then be generated to synchronize the designators (and any other unmatched component properties).
• Cancel - click this button to generate ECOs to add extra components that are present in the source editor and remove extra components from the target editor.

Manually Linking Components

The status of the component links can be checked and managed at any time, in the Edit Component Links dialog (PCB editor, Projects » Component Links command).

Summarizing the dialog features:

• 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 arrow buttons in the middle of the dialog are used to manually match (or un-match) selected components.
• The Add Pairs Matched By button and options down the bottom of the dialog are used to scan the list of currently unmatched components, and attempt to match them by the enabled properties (Designator, Comment, Footprint).
• When the Perform Update button is clicked, each newly matched PCB component is assigned the UID of its schematic counterpart.
• After using this dialog to perform manual component linking, it is good practice to check the synchronization state (run the Design » Update command).

The Edit Component Links dialog is used to detect and resolve UID mismatches, it is 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.

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

• During design synchronization, the default behavior is to first attempt to match by members, in accordance with the Min Match % and Min Match Member settings.
• If member matching fails, the software will then attempt to match by name (if the Use Name Matching option is enabled).
• If either of these matching processes succeeds, you will proceed to the Engineering Change Order dialog.
• If both matching techniques fail (or the Use Name Matching option is set to Never), the Match Manually dialog will open.

• 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.
• If you click Yes in the dialog to match manually, the Match dialog will open, as shown below (the dialog caption will change 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.

• In this dialog, select the objects that you want matched in the Unmatched Reference Objects and Unmatched Target Objects, and then transfer them to the Matched Pairs section of the dialog. For these objects, the software will generate an ECO to update the names so they now match, and ECOs to remove/add members, so they also match.
• If you are unsure, you do not have to manually match objects. For any unmatched objects, the software assumes that the reference and target objects are unrelated, so will generate ECOs that remove the Unmatched Reference Objects from the board, and add the Unmatched Target Objects as new objects.
• Once you have matched those objects that you know do match, click Continue to open the Engineering Change Order dialog.
• If you click Cancel, the update process terminates.

Matching the Design Rules

Design rules that are defined on the schematic must also be linked to the matching rule on the PCB. If there was no linking mechanism, you would not be able to update the rule on the schematic and flow those changes to the PCB. UIDs are used to link the schematic design rule to the PCB design rule.

The UID is automatically assigned in the Parameter Set that holds the rule definition on the schematic, 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.

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.