Applied Parameters: ObjectKind=Project|Action=VariantManagement
This command is used to run the Variant Management dialog, from where you can add, remove and edit variants for the active PCB design project. The ability to create variations of the same base design is a real strength of Altium Designer, and a tremendous productivity booster for designers. Using variants, you can define any number of variations of the base design, configuring each component to be: fitted; not fitted; fitted with modified component parameters, such as the component's value; or you can completely replace a component with an alternate part. Variants that use any of these types of variations are all referred to as Assembly Variants, as they only impact on the assembly process - all variants share the same fabricated bare board. There is also support for variations to component overlay information on the PCB, for example changing a component's comment. This type of variation requires two overlay screens to be produced, resulting in two different bare boards. This type of variant is referred to as a Fabrication Variant.
For an in-depth walk-through of Altium Designer's capabilities with respect to variants, see Design Variants
This command is accessed from the Schematic Editor, and PCB Editor, by choosing the Project » Variants command, from the main menus.
First, ensure that a source schematic, or PCB document, for the project whose variants you wish to manage, is open as the active document in the main design window.
After launching the command, the Variant Management dialog will appear. The dialog presents two distinct regions of information:
- Components - lists all of the components in the base design.
- Component Parameters - details all of the parameters of the component(s) currently selected in the upper region.
Use the dialog to create variants of the original (base) design, and determine how each is populated, in terms of its components, in order to create different (varied) products as required. The following component variations are supported:
- Fitted - this is the default state of a component, if it is Fitted, then it is not varied. When you create a new variant, all components default to Fitted. A component with a state of Fitted is represented in the Variant Management dialog as an empty cell.
- Not Fitted - if a component is set to Not Fitted, it still exists on the schematic and is transferred to the PCB, but it is removed from the appropriate output documentation, such as the BoM. For a Not Fitted component the cell displays the text Not Fitted. You can also configure how Not Fitted components are presented in the documentation, for example they can be marked with a cross on the schematic and in PCB drawing outputs.
- Alternate Part - it is also possible to select an entirely different component, as an Alternate Part. Once chosen, the cell displays the alternate part's Library Link. Since the Alternate Part is a different component, only one or the other component is presented on the compiled tab of the compiled schematic sheet. There is also the requirement that the alternate part shares the same set of pins, placed in the same locations, as the base part. This is an essential requirement to ensure the connectivity remains valid when the design is compiled.
After selecting an alternate part, the software checks for pin-compatibility between the chosen alternate component, and the original base design component. To be pin-compatible, the alternate must have the same number of pins as the original component, and those pins must be identical in their location, and electrical type. No equality in the graphical primitives used in the symbols for the two components is required. If the software detects that the alternate component is not pin-compatible, a Confirm dialog will appear, requiring your OK to proceed with the replacement. While you can proceed with the use of a pin-incompatible alternate component, bear in mind the potential impact on the wiring, and that you may also encounter an error violation when performing a subsequent compilation of the design.
In addition, you can also vary any of a fitted component's parameters. Modifying the value of a parameter is a local variation, only affecting the output documentation. The original schematic, and the component whose parameter is being varied, are not modified in any way.
Once variants and their configurations have been defined as required, click OK to save those configurations.
- Once a variant has been added for a project, a Variants folder will appear directly below the project's entry in the Projects panel. The folder contains all currently defined variants, as well as the base design ([No Variations]). Double-click an entry to make that the active/current variant. The Variant Management dialog can also be accessed by right-clicking on the Variants folder and choosing the Variants command from the contenxt menu.
- To examine design variations, you must compile the design and then switch to the compiled tab of the schematic (thereby viewing the physical design). Choose the required variant from the Variants folder for the project, in the Projects panel, to show the configuration of the physical components on that sheet.
- Alternate part variations within a specific channel of a multi-channel design are not supported. If you choose to use an Alternate Part, it must be used in all channels.
- Double-click on a component in the Variant Management dialog to jump to that component on the schematic.
- It is often easier to work directly from the component(s) placed on the schematic sheet, rather than scrolling up and down through a list of components in a dialog. Simply select the component(s) on the sheet, then right-click and select Part Actions » Variants from the context menu. The Variant Management dialog will open, displaying only the selected components. In addition to only presenting the selected component(s) in the Variant Management dialog, if there is a variant currently selected (in the Variants folder for the project, in the Projects panel), then only that variant will be presented, irrespective of how many variants might actually be defined for the project.
- Variant settings are stored in the project file (
*.PrjPcb). When the Variant Management dialog is opened, this data is read and analyzed, then loaded into the Variant Management dialog. If there are issues detected during data loading, such as mismatches between component designators or component UIDs, an Information dialog will open outlining the problem. Component UID mismatches are automatically resolved, simply close the dialog and save the project to retain these corrections. Duplicate designators must be resolved at the schematic level, recompile the project and check the Messages panel for warning/error details to resolve these.
- There are two ways an Alternate Part is handled on the PCB:
- If the footprint is the same - if the chosen Alternate Part has the same footprint name as the base part, then only one instance of that footprint will be transferred to the PCB. As multiple footprints can be assigned to a component, you should ensure that the correct footprint is selected in the Variant Management dialog for each variant.
- If the footprint changes - if the chosen Alternate Part has a different footprint name from the base part, then both footprints are transferred to the PCB. As the designer you must then decide how to position the two footprints on the PCB. Note that both footprints will have the same designator, as only one or the other component is ever fitted.