Working with Components Placed on Your Schematics in Altium Designer

A component within a library represents the physical device that is placed on the actual printed circuit board. On a schematic sheet, a component is represented by its schematic symbol model. Each component can contain one or more parts.

Updating and Replacing Components from a Library

Having initially placed components onto schematic sheets of a board design, there now needs to be some way of updating those component instances, with any changes to their linked source components in the applicable Workspace. In other words, a means by which to keep the design synchronized with the Workspace entities that it uses.

For example, a component may have been re-saved to the Workspace, perhaps reflecting a change to a child model. This results in a new revision of that component. The placed instance of that component is now using an older revision and you may want to update it to use the latest revision instead. Alternatively, you may have decided to use a different component altogether, and simply need to change the existing component in the design for an alternate one.

This page outlines updating a component placed from your connected Workspace. For information on how to update a component placed from a database or file-based library, refer to the  Updating Components from Database and File-based Libraries page.

There are various methods available by which to manage the components after initial placement into a design.

Single Instance Component Change

Each placed component has a link back to the component revision in the Workspace. This information can be found on the Properties panel, when browsing the properties for the selected component.

Each placed instance of a component has a link back to the specific revision of that component in the Workspace.Each placed instance of a component has a link back to the specific revision of that component in the Workspace.

If there is a later revision of the existing component available, the entry for the revision status (on the Properties panel) will reflect this using the text Out of date, to the right of the current revision's lifecycle state. Note that if the lifecycle state has been marked as not being allowed for design (Allowed to be used in designs option disabled for it in the State Properties dialog), then the entry will instead show as Inapplicable.

At this lowest, individual component level, the placed instance can be:

  • Updated to the latest revision of the existing component, by clicking the button.

Example of updating the same component to its latest revision – hover over the image to see the result.Example of updating the same component to its latest revision – hover over the image to see the result.

  • Switched out for the latest revision of a different (a replacement) Workspace component or a file-based library component by clicking the button at the right of the Design Item ID field. The Replace Component dialog will open, presenting components in your connected Workspace and available file-based libraries. The current component is shown at the top of the list. Search for the replacement component required, select it, then click OK.

    Example of replacing the existing component with a different one (an alternate)Example of replacing the existing component with a different one (an alternate)

    The Replace Component dialog provides direct access to all available Workspace library components and file-based library components. The dialog offers full details of the selected component (Parameters, Models, Part Choices, Supplier data, etc.,), component comparison, and for Workspace Library Components, a filter-based parametric search capability for specifying target component parameters.

    The Replace Component dialog can also be accessed from other places of Altium Designer when performing a component replacement operation, e.g. from an ActiveBOM document or the Item Manager dialog.

Effecting Batch Component Changes – the Item Manager

Related page: Managing Content with the Item Manager

Individual component change is great, however, it soon becomes tiresome when dealing with a more sizable number of components. For this, you need a single, centralized place from which to effect multiple changes in a batch-like manner. Enter the Item Manager (Tools » Item Manager).

The Item Manager is 'command-central' for synchronizing Workspace design entities – placed on schematic sheets – with the source content they are linked to in a Workspace. It automatically detects and lists all components, flagging if they are Workspace entities or not, and then compares the Item-Revision of each Workspace component on the schematics against the available revisions of that component in the Workspace. For each entity, information about the current linked Item is given, in terms of revision, lifecycle state, and the source Workspace in which it resides.

The automated comparison of revisions for Workspace content flags any that is out of date. That can then be selected and prepared for update to the latest revision with minimal effort. For more detail, see Detecting when Updates are Required.

You have full control over which of these Workspace entities to update, and how. For example:

  • Select an individual entry and update it to use the latest revision of the linked Item, or choose to use the latest revision of a completely different Item.
  • Select a group of entries that utilize the same linked Item and either update them to the latest revision of that Item, or choose to use the latest revision of a completely different Item.

All proposed changes are reflected in the manager.

Once changes have been set up as required, generate an Engineering Change Order (ECO) and browse the actions that will be taken to implement those changes. Disable any actions if required – you are always in the driving seat! When ready, execute the ECO and the changes will be affected. Fast and efficient, your placed Workspace content is managed with simplistic ease.

If you're confident in the changes you are making, you can use the Item Manager's Apply ECO feature – effecting the changes quietly, without popping the Engineering Change Order dialog.

The following examples illustrate use of the Item Manager:

  • To update multiple components to use the latest revision of the existing Workspace component.

Update a group of out-of-date components to their latest revisions.
Update a group of out-of-date components to their latest revisions.

  • To change a couple of components for the latest revision of a different Workspace component – chosen through the Replace Component dialog.

Replace one or more components with a different Workspace component.
Replace one or more components with a different Workspace component.

Not only can the Item Manager be used to keep your components in your designs in sync with changes to the source content in the connected Workspace(s), it is also a powerful tool to aid in the migration of your existing board designs – from using local design items to using Workspace design content. Once you have migrated your design components to a Workspace, and any schematic sheets (device sheets), you use the Item Manager to 'replace' the existing components and sheet symbols with their newly migrated Workspace incarnations. In other words, the components remain the same, from the design perspective, but the source of those components changes.

Powerful auto-matching capabilities enable you to quickly match local components and sheet symbols to Items in the Workspace.

Changing a Component from a BomDoc

It's not uncommon to identify an issue with a component when the BomDoc is being checked and made ready for ordering the parts. For example, the designer may have forgotten to finalize the selection of a component, or a component has gone EOL and the designer wants to explore the price and availability of potential replacements. While you could resolve this by returning to the schematic and editing the component, selecting a suitable part, then refreshing the BomDoc, ActiveBOM supports performing this directly from within the BomDoc – then pushing that change back to the schematic via an Engineering Change Order.

From within the BomDoc, right-click on the selected component(s) and select the Operations » Change <ComponentName> command. The Replace Component dialog will open, from where the replacement component can be searched for. After finding the desired replacement component select it, then click OK. The Engineering Change Order dialog will open, detailing the changes needed to synchronize the schematic with the BomDoc.

Example of component replacement directly from within a BomDoc.
Example of component replacement directly from within a BomDoc.

  • The replace component feature searches for a new component in the currently active Workspace.
  • If the component change also affects the board design, an update to the PCB should also be performed from the schematic.
  • The Replace Component dialog has a similar layout and shares many of the features with the Components panel

Replacing a Generic Component

When a design has progressed to the point where a Generic Component can be replaced with a specific physical component, invoke the Replace Component dialog by selecting the button in the Properties panel. Note this also can be done from the Item Manager or through the project's ActiveBOM document.

Parameter values that have been applied to the Generic Component (here, power and resistance values) are automatically used as search terms in the Replace Generic Component dialog, allowing you to choose a suitable replacement component from the filtered results – in the example case here, two component entries fit the search criteria.

Replacing a Generic Component through the Properties panel. Hover the cursor over the image to see the result.
Replacing a Generic Component through the Properties panel. Hover the cursor over the image to see the result.

Note that the component replacement logic also supports multiple selections. When a number of generic components are selected for replacement via the Properties panel, the manufacturer component chosen in the Replace Generic Component dialog will replace all of those selected components.

Managing Footprints Across the Entire Design

Altium Designer's Schematic Editor includes a powerful Footprint Manager. Launched from the Schematic Editor's Tools menu (Tools » Footprint Manager), the Footprint Manager lets you review all the footprints associated with every component in the entire project. Multi-select support makes it easy to edit the footprint assignment for multiple components, change how the footprint is linked, or change the current footprint assignment for components that have multiple footprints assigned. The Footprint Manager facilitates reviewing and detecting problems with footprint assignments across the entire design, particularly useful when you are working on a legacy design or one from another organization. Design changes are applied through the ECO system, updating both the schematic and the PCB if required.

The Footprint Manager dialog presents a list of all components across all source design schematics in the active project. Use the controls available on the right-hand side of the dialog to manage the footprints available to, and in current use by, the design's components. Features include:

  • Ability to add, edit, and remove footprint models for one or more selected components.
  • Copy footprints between components.
  • Changing current footprint assignment (the footprint that will currently be used to represent a component in the PCB domain, from multiple that may be available to that component).
  • Footprint validation - to ensure that footprint models are truly available, and especially those set to be the current model.

Once all changes to footprint model assignments have been made as required, those changes are then implemented through a standard Engineering Change Order (ECO). To do this, simply click on the Accept Changes (Create ECO) button, at the bottom-right of the Footprint Manager dialog.

For a design containing device sheets, the components on those sheets will only be listed provided the sheets are not marked as being Read-only. Toggle the Read-only state for device sheets in projects from the Data Management - Device Sheets page of the Preferences dialog.
If the design has been captured using a range of libraries and the footprints have been manually attached or edited, it is imperative that a careful review of all footprint data is undertaken. The Footprint Manager can be used to help rationalize footprints across the design, but some level of sanity checking will also be required. There is no way for the system to catch design errors, such as specifying a 20W resistor onto a 0603 footprint. These all need to be reviewed carefully, and recognize that footprint names can vary across component suppliers. Do not assume anything!
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Note

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.

Content