Contact our corporate or local offices directly.
Parent page: Design Variants
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.
As previously outlined, the actions to examine variant detail on the schematic are:
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.
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.
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.
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
Not Fitted state of a component for the variant design. Launch this command using the button on the Variant Active Bar (available when a variant is selected in the Projects panel).
Not Fittedstate of the selected components.
The component’s fitted state will be graphically indicated as defined in the Variant Options dialog.
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.
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.
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.
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.
Enable the Annotate option to specify either:
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.
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.
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:
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:
► Learn more about working with variants in ActiveBOM
Assembly variants affect all output documentation that includes detail about the purchase or loading of components. This includes:
Fabrication variants also affect the following outputs:
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.
If the output is generated via another interface, for example, the Report Manager or an OutputJob, it will include a Variant selector.
Main article: Preparing Multiple Outputs in an OutputJob
There are two approaches to configuring an OutputJob file to support 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.
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.
► See Preparing Multiple Outputs in an OutputJob for more information on Variants in Output Jobs
Contact our corporate or local offices directly.