Contact our corporate or local offices directly.
Parent page: Design Variants
Variants are created and configured in the Variant Management dialog. To open the dialog, select Variants from the Project menu (shortcut: C, V).
The dialog has two main regions:
Click the button in the Variant Management dialog to create a new variant of the base design. The Edit Project Variant dialog will open, enter a name for the variant in the Description field and click OK. The other options in this dialog are discussed in more detail later.
An additional column will then appear on the right of the Variant Management dialog, with the new Variant name as the column title. All the cells will be empty, where an empty cell indicates that this component is Fitted and unchanged from the base design. The components can now be configured for the new variant. The image below shows a project that has had two variants created, BGA and TSOP.
The Variant Management dialog includes a number of interface features that assist the display of useful information. These are configured via the right-click context menu.
Useful commands include:
Once the Variant itself has been created, the state of each component is ready to be varied. This can be done by clicking the component cell in the variant column to reveal the control, or by right-clicking on a non-selected cell to access the context menu Set Selected As sub-menu.
The control opens the Edit Component Variation dialog which (along with the Set Selected As sub-menu) offers three choices:
When the Alternate Part option is selected, the Edit Component Variation dialog expands to show the base parameters of the existing part. Use the button to browse and locate the required alternate part component in the Replace Component dialog – a modal dialog version of the Components panel. All of Altium NEXUS's component storage models are supported, such as independent libraries, database libraries, as well as server-based components (as shown in the example below).
The newly applied alternative component can be checked back in the design space. In the applicable schematic sheet for that component, switch to the compiled tab view and then select the required variant in the Variants section of the project, in the Projects panel.
The Schematic Editor will use the symbol graphics for the alternate component, however, if the component is pin-compatible and graphically similar there may be little noticeable change.
To help make it easy to visually identify varied components, the color and font of varied parameters (such as the component comment string), can also be varied. This is configured in the Variant Options dialog. Click Drawing Style in the Variant Management dialog to open the dialog. Note the green italic font used for the alternate component in the animation below.
If a base component uses a graphical display mode other than the default
Normal Mode, and it also has an alternate component defined in a variant, then the alternate component will attempt to use the same graphical display mode. Conversely, if the alternate component does not include this graphical display mode, then the
Normal mode is used.
Part view Modes are defined in the Schematic Library Editor with the Component Display Mode commands and are selected for a placed component in the Graphical section of the Properties panel, as shown below. In this example the base part symbol uses Mode,
Altium NEXUS supports several ways of storing and working with components, including the use of a DBLink file with the project. A DBLink file is an interface between the components on the schematic and a company database.
Rather than just creating a reference from each component to a specific database record (as is typically done when you place a component from a DBLib-type library), the DBLink model relies on the designer initiating a query action based on one or more component parameters. The software then searches the database for a record with fields that contain matching values, and when a match occurs, other field values from that record (such as the Part Number) can be returned to the Altium NEXUS component. The component parameter-to-database field mapping is defined in the DBLink document, as is the target database.
► Learn more about Working with Database Libraries
In a design that does not use Variants, the query action is performed via the Update Parameters from Database command, and can also be performed during BOM generation by enabling the Include Parameters from Database option (see below), to extract BOM-specific component data, such as price.
For a design that includes Variants, the parameters used to query the database are varied in the Variant Management dialog. Since those parameter values only exist in the Variant Management dialog, the Update Parameters from Database command is not used to retrieve database information – instead the parameters are extracted from the database when the BOM is being generated.
The Variant Management dialog includes features to help control the amount of data displayed, which is particularly useful when working on a large design.
The way in which varied components are presented in schematic design documents (and PCB outputs) is configured in the Variant Options dialog. Those settings subsequently affect how the component variations are presented in printed or PDF outputs, and in PCB printouts such as Assembly drawings. To access the Variant Options dialog, click at the bottom of the Variant Management dialog, after selecting a cell in the relevant variant column.
Design variations set up in the Variant Management dialog are ultimately saved in the project file. This includes the Not Fitted state, local parameter variations to a Fitted component, and the parameter values of Alternate Parts. The actual Alternate Parts are stored in a [ProjectName].PrjPcbVariants file. The Variant Management dialog includes commands for resetting parameters and updating components, which helps to ensure that they are in sync with the source component libraries.
Parameters modified locally in the Variant Management dialog can be restored to their original value by right-clicking on the modified parameter (shown in bold) in the Variant Parameter list, and then choosing Reset Selected from the context menu – as shown below. Note that multiple parameters can be selected at once then reset in a single action, or Reset All used to reset all parameters for that component.
If a library component that is used as an Alternate Part has had parameters changed in the library, then you to can bring those changes directly into the variant definitions in your project by right-clicking in that Variant's Parameter list and selecting Update Values from Library from the menu (as shown below). Note that this updates the parameters, if you need to update the graphic, use the technique described below.
Following the Update Values from Library command, browse to and locate the component in the source library or Managed Component Server (via the Browse Libraries dialog or the Server content Explorer) and click OK to open the Update Project Variants From Library dialog. Select/deselect the Parameters from Library Component and Variants to Update, then click OK to complete the update process.
All parameters are listed on the left of the Update Project Variants From Library dialog – if required, any parameter can be deselected to exclude it from the update process. On the right of the dialog, the target Project Variant can be changed (Project Variant To Update). This will default to select the Variant that was selected when the Update Values from Library command was activated.
If the source component for an Alternate Part has been edited in its library, it can be updated in the design by running the Update from Library dialog.
Launched from the Tools menu in the schematic editor, the dialog includes an option to Include Variants. When this option is enabled, the component list will expand to include any components that have been used as Alternate Parts. Check the components in the list to be updated, and then complete the Wizard to update the required parts from the source.
The Variant Management dialog supports multi-select, which means that any number of components can be selected simultaneously in the upper (Component) part of the dialog, and then updates performed on any number of parameters selected in the lower (Parameters) part of the dialog. The dialog also offers Filters (via the right-click context menu), to further refine the selection and the displayed data.
By way of example, to reset the manually-varied parameters for all components, in all variants:
If you have been experimenting with the Filter options and have applied different filters, you may need to reset the filter before attempting another update. To do this, disable the Only Show Varied Components option to clear the filter system, then re-apply it and clear the Filter options as required.
Altium NEXUS supports Parameters at various levels of a project. For example, document-level parameters can be added to each schematic sheet in the Parameters tab of the Schematic editor Properties panel (available when nothing is selected). Project-level parameters can also be added to a project on the Parameters tab of the Project Options dialog (Project » Options). Further to this, parameters can also be added to a Variant via the Edit Project Variant dialog. In the Variant Management dialog, select the variant column and click the Edit Variant button to open this dialog.
Parameters included at various levels in a project exist in a hierarchy, which means you can, in fact, create a parameter with the same name at different levels in the project, where each has a different value. Altium NEXUS resolves this situation using priorities, in the following way:
This arrangement means that the parameter value defined in a schematic document overrides the value defined in the Project options, and the parameter's value defined in a Variant overrides the value defined in the schematic document. Note that schematic-level parameters are not available on the PCB or in the BOM – for these types of output, project or variant parameters should be used.
In the images below, a Parameter called
ProjectTitle has been defined for the project, and also for each variant. The animation shows the behavior on the PCB as the Variants selector is used to show the base design, then each variant.
Variant settings are stored in the project file (
*.PrjPcb), and this data is read, analyzed and loaded into the Variant Management dialog when that dialog is opened. If issues are detected when the data loads, such as any mismatches between component designators or component UIDs, an Information dialog will open to outline the problem.
Component UID mismatches are automatically resolved, and these corrections will be retained when the project is saved. Duplicate designators must be corrected at the schematic level. To resolve these, validate the project (Project » Validate <project name>) and check the Messages panel for warning/error details.
Contact our corporate or local offices directly.