Working with Variants in the Design in Altium NEXUS

Created: July 12, 2022 | Updated: September 2, 2022
Applies to altium-nexus version: 5
This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer (with Altium Designer Enterprise Subscription) and a connected Altium 365 Workspace. Check out the FAQs page for more information.

Parent page: Design Variants

Working with Variants in the Schematic Editor

Altium NEXUS's schematic editor includes a range of features that provide full visibility of component variations during the schematic capture process, as described below.

Examine Varied Components

As previously outlined, the actions to examine variant detail on the schematic are:

  • Select the required variant in the Variants section in the Projects panel by double-clicking on its entry or by on the desired variant and selecting the Set as current command.
  • Select the named compiled tab located at the bottom of the schematic sheet.
  • Components varied on the sheet will then be displayed, in the style configured in the Variant Options dialog.

Examining the varied components on the schematic
Select the variant and then the compiled sheet to view the components that are varied on a schematic sheet (identified by their varied parameters).

The compiled tab displays a different Active Bar at the top of the design space, which includes variant-specific buttons. These buttons are only available when a variant is selected in the Projects panel.

Note that when you switch to a compiled tab the available menu entries will change, reflecting the commands that can be run when you are viewing the physical design. Click on the logical design tab (Editor) at the bottom of the schematic sheet to return to the standard editing menus.

Selecting Variant Components from the Schematic

As opposed to scrolling through and selecting components from the list in the Variant Management dialog, it can be more convenient to make specific selections directly on the schematic. To do so, select the component(s) on the sheet, then right-click and select Part Actions » Variants from the context menu.

Modifying the variant properties of components selected on the schematic
Here, two components (LEDs) have been selected on the compiled tab of the schematic for the BGA variant – the right-click Variant command will open just those components in the Variant Management dialog.

Note that the right-click Part Actions sub-menu also includes commands to Toggle Fitted/Not Fitted, and to Choose Alternate Part.

The Variants command on the right-click menu (above) will open the Variant Management dialog, where only the selected components will be listed. The required variations can then be performed as usual and OK clicked to apply those variations to the design.

Variant Management dialog, opened to display only the components selected on the schematic
Here, the Variant Management dialog has been opened from two selected components on the schematic sheet and therefore includes just those two (LED) components.

This selection technique can be used when first setting up component variations, or when an existing component variation needs to be modified. 

Graphically Editing Component Variations

Component Variants can also be created and edited by working directly in the schematic at a symbol level. Note that the Schematic Editor must be in compiled variant view (as selected by the lower tab), and the required variant selected in the Projects panel.

A command is provided to quickly toggle the Fitted or Not Fitted state of a component for the variant design. Launch this command using the Toggle Fitted State button button on the Variant Active Bar (available when a variant is selected in the Projects panel).

  • When no component is selected in the design space, this will change the cursor to a cross-hair, where clicking on a component will cause it to toggle between the Fitted and Not Fitted states.
  • When there are components selected in the design space, clicking the button will toggle the Fitted / Not Fitted state of the selected components.

The component’s fitted state will be graphically indicated as defined in the Variant Options dialog.

Graphically editing component variationsToggle a specific component's fitted state directly on the schematic.

Graphical Parameter Editing

Changes can be made directly to a displayed component variant parameter by selecting the parameter text then clicking the text a second time to enable editing mode. Any changes made will be adopted by that component’s entry in the Variant Manager dialog.

Note that a component’s parameter visibility is configured in the Properties panel. With a component parameter selected, use the icon associated with the parameter Value to toggle its visibility.

Graphically editing parameter variationsSelect a parameter, then click a second time to enable direct editing.

A variant parameter may also be directly edited in the Parameter Variation dialog, which is opened by double-clicking on the parameter text. As usual, this function is only available when in the compiled schematic view, and any changes made will also register in the Variant Management dialog.

Editing parameter variations in the Parameter Variation dialogWhen in the compiled view, double click on a variant parameter access editing in the Parameter Variation dialog.

Graphical Designator Editing

To change a component's physical designator, directly within the compiled document view of a source schematic, simply click once on the designator to focus it, then click again to begin editing. Note that in-place designator editing is only possible when the Enable In-Place Editing option is enabled in the Schematic – General page of the Preferences dialog.

Graphically editing a component designatorSelect the designator, then click a second time to enable direct editing.

In-place editing of designators is essentially a graphical shortcut to defining a Locked Physical Designator, which can also be defined in the Physical Component Properties dialog by double-clicking on the component.

The Physical Component Properties dialog gives access to designator editing and annotation options for variantsBoth the associated component and designator dialogs provide access to designator editing and annotation options.

Enable the Annotate option to specify either:

  • A custom designator, using the Lock Physical Designator option and entering the new designator. This is the option that is set when graphically editing a designator, as outlined above.
  • A designator generated using a specified Naming Scheme. In this case, enable the Apply Naming Scheme option and use the Annotate Options button to access the Board Level Annotation Options dialog. From here, you can either choose a predefined naming scheme or specify your own, custom scheme. The Physical designator will be generated based on the logical designator information and the specified naming scheme.

Refer to Annotating the Components for detailed information on Annotation and Naming Schemes.

The options defined in the Board Level Annotation Options dialog when defining a naming scheme are global to the project and override the naming scheme defined on the Multi-Channel tab of the Project Options dialog (Project » Project Options).

Working with Variants in the PCB Editor

In Altium NEXUS's PCB editor all of the component footprints, for all variants, are always shown. This is necessary because all footprints, for all assembly variations, must be fabricated as part of the bare board. It is the loading of components during the assembly process that then determines which variant is being built.

Because all footprints are always visible on the PCB, it can be difficult to know which components belong to which variant. However, the only visible clue to tell if a particular component is fitted or not fitted in that variant is if the component includes a 3D Body model. The body will appear/disappear to indicate whether the component is fitted or not fitted. This visual behavior is more easily seen when the PCB is in 3D Layout Mode as demonstrated in the animated image below.

Alternate Part PCB design

There is only one type of variation that affects component placement in the PCB design process – when an Alternate Part is specified, and that Alternate Part uses a different footprint from the base design. In this situation, two footprints must be placed on the board.

There are different ways that these two footprints might be positioned, such as:

  • The footprints are placed next to one another.
  • The smaller footprint is placed inside the larger footprint, as shown in the animation below, where an SRAM component is available in either a TSOP package or a BGA package.
  • The footprints are exactly stacked (placed one on top of the other). For example, when the footprints are identical but have different 3D models, and therefore must have different footprint names. This is also shown in the image below, where two LED footprints are stacked for both DS1 and DS2.

Demonstration video, how varied components, that use different footprints, can be placed on the board A simple animation showing how Alternate Parts that use different footprints can be positioned on the board.

PCB components that share the same footprint but different 3D models, can be stacked on the board
The two instances of LED DS1 use exactly the same footprint pattern (but have different 3D models in each variant) and can therefore be stacked.

Altium NEXUS includes design rule checking support for stacked alternate components, so no additional design rules are required. The alternate parts share the same component UID, however, the software is aware that they are alternate parts and can prevent the rules engine from flagging stacked or overlapping alternate-part footprints.

Working with Variants in ActiveBOM

Main article: BOM Management with ActiveBOM

Although a BOM can be generated directly from the schematic or from an OutputJob file, the recommended approach is to use ActiveBOM. Beyond the components fitted to the board, ActiveBOM allows additional components and BOM-specific data to be added directly in ActiveBOM, for example; yet-to-be-detailed parts, fasteners, the blank board, or the mounting glue. Custom columns can also be added, including a specific Line number column, which supports both auto and manual numbering, with full copy/paste support.

For design components that include manufacturer information, ActiveBOM can use the Altium Cloud Services to access detailed and up-to-date supply chain information. This support extends beyond components placed from a managed content server, also supporting Supplier-linked parts, as well as parts that already have suitable manufacturer details in their parameters.

ActiveBOM supports variants in the following ways:

  • Display the BOM for a specific variant in Base view mode or Flat view mode
  • Option to include the Not Fitted items in the BOM Items list
  • Display a consolidated list of all parts used in all variants, in Consolidated view mode
  • Define manual solutions for both base components and varied components

ActiveBOM includes a consolidated view mode, use this to include all parts used in all variants, into a single BOMActiveBOM includes a consolidated view mode, allowing a single BOM to detail the parts in all variants.

Learn more about working with variants in ActiveBOM

Variant Output Generation

Assembly variants affect all output documentation that includes detail about the purchase or loading of components. This includes:

  • Bill Of Materials (using ActiveBOM or directly via the Report Manager)
  • Schematic Prints
  • PCB 3D Prints
  • PCB 3D Videos
  • Assembly Drawings
  • Pick and Place files
  • Test Point Report

Fabrication variants also affect the following outputs:

  • Gerber overlay layers
  • ODB++ overlay layers

Selecting the Variant for Output

If you are running a command from the schematic editor or PCB editor, such as a schematic printout or Gerber files generated directly from the PCB editor, the output will be generated based on the variant currently selected in the Projects panel.

Select the variant in the Projects panel before generating output from the schematic or PCB editor menusOutput generated directly from the schematic or PCB editor menus is based on the variant selected in the Projects panel.

If the output is generated via another interface, for example, the Report Manager or an OutputJob, it will include a Variant selector.

Output interfaces, such as the Report Manager or the OutputJob editor, include variant selection featuresRight-click in the Report Manager to switch from one variant to another.

Working with Variants in the OutputJob Editor

Main article: Preparing Multiple Outputs in an OutputJob

There are two approaches to configuring an OutputJob file to support variants:

  • Choose a single variant for the whole OutputJob file – use this when you prefer to use a separate OutputJob for each variant, or
  • Choose a different variant for each output – use this when you have a single OutputJob configured to generate outputs for multiple variants.

The option is selected in the Variant Choice region of the OutputJob editor. When the second option is enabled the required variant must be selected for each output that supports Variant-type output, as shown in the image below.

In the OutputJob editor you can select a variant for all jobs in the file, or individually select the variant for each job
An OutputJob where the Choose a different variant option is selected and outputs for both variants have been set up for each Job in the OutputJob file.

If the first 'blanket' approach is used, then every output file that is variant-specific will automatically be configured for that variant. The advantage of this option is that the variant does not need to be specifically selected, whereas the disadvantage is that an OutputJob file is required for each variant in the design.

If Fabrication Variants need to be generated from the design, enable the Allow variation of fabrication outputs option in the Edit Project Variant dialog. If an output job has a variant nominated for a fabrication output, and that variant does not have the option enabled, the job's variant name will be displayed in red.

Note that the red variant name is simply a warning flag, and the variant-specific output files will still be generated. If a fabrication variant is not required, ensure that the Variant dropdown menu for that output job is set to [No Variations] – in this mode, the output will be generated from the base design.

If Paste Mask outputs need to be generated for a design that includes variants with 'Not Fitted' components, enable the Allow variation for paste mask option in the Edit Project Variant dialog. These components will no longer have Paste Mask openings included on their pads.

See Preparing Multiple Outputs in an OutputJob for more information on Variants in Output Jobs

Viewing Variants in the Web Viewer

Design variants are also supported when viewing the project in a Workspace's Web Viewer.

To learn more, refer to the Variant Support section of the Web Viewer page (for an Altium 365 Workspace or NEXUS Server Workspace).

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: