The Components panel provides direct access to available Workspace components, and database and file-based library components in Altium Designer.
The panel sources components from a connected Workspace and any open or installed libraries. The panel offers full details of the selected component (Parameters, Models, Part Choices, Supplier data, etc.), component comparison, and for Workspace components, a filter-based parametric search capability for specifying target component parameters.
The Components panel uses the basic search engine functionality and view that is applied in the Manufacturer Part Search panel. While the Manufacturer Part Search panel harnesses the Altium Parts Provider service and focuses on the component manufacturer and supplier data searches, the Components panel is populated with ready-to-place components from your connected Workspace and database and file-based library sources.
To open the Components panel, select View » Panels » Components from the main menus or the Components option from the button menu at the lower right of the main screen. Using a responsive design configuration, the panel layout will dynamically adapt between full-screen normal mode () and its compact mode () where the Categories/Filters options collapse to menus.
From within a schematic document, use the P, P keyboard shortcut to open the Components panel. From within a PCB document, use the P, C keyboard shortcut.
The panel’s Categories pane (or the drop-down menu in compact mode) lists all available Workspace components under the All category entry and any available libraries. When the panel is in its normal mode, click the Categories list icon or the « icon to collapse or expand the display of the column and use the button (top right) to toggle the visibility of the component Details pane. When sifting through the Categories pane, the Up/Down and PgUp/PgDn keyboard shortcuts may be used to walk through the list. The Left/Right keyboard shortcuts may be used to open and close the individual branches.
The operations menu options provide you the ability to set file-based libraries preferences, perform searches, and specify if component models collection is visible. To access these options, select the operations menu button at the top right of the panel.
Select the File-based Libraries Preferences command from the menu to open the Available File-based Libraries dialog, where you may view controls to add or remove libraries, install libraries, and specify library search paths. The Available File-based Libraries dialog has three tabs and is described in the following sections.
This tab lists all of the libraries that are part of the active project (the project currently selected in the Projects panel).
To add a library to the project, click the Add Library button. A dialog will open in which you can browse to and select a library file that you want to add to the project.
The following types of library files are supported as project libraries:
*.PcbLib) – only viewable if the Footprints option is enabled from within the Libraries menu.
Use the Move Up and Move Down buttons to define the search order of the libraries.
This tab lists all of the installed libraries. This list is an environment setting. Any libraries added to the list will be available for all projects and the list is persistent across design sessions. Project libraries can be added to this list but are not initially part of it.
Click the Install button then select Install from file to open a dialog in which you can select the desired library you want to add to the list.
The following types of library files are supported as installed libraries:
Use the Move Up and Move Down buttons to define the search order of the libraries.
This tab lists all libraries that have been found along the Library Search Paths for the project. These paths are defined in the Search Paths tab of the Project Options dialog. Click the Paths button to open the Search Paths tab to define further search paths or modify existing ones as required.
Use the Refresh List button to update the search paths and ensure that the library list is current.
Libraries in this tab are searched in the order they appear. Click the Paths button to define the order. Search paths can be defined as a specific file or to a folder, including subfolders.
When you do not know which file-based library contains a component or if it is even available, you can search for it. To search for a component, select the File-based Library Search option from the libraries menu () at the top of the panel to open the File-based Libraries Search dialog.
The searching process can be summarized as follows:
The Filters region is used to define text strings that are to be applied to searching. There are three regions to configure:
There are essentially two approaches to searching:
Searching will return all items of the chosen search type (Components/Footprints/PCB3D Models) found in all libraries that fall under the defined Scope (Available Libraries/Libraries on path on the specified search path). For example, if you want to find a component that you think is in a library within specific folders on the hard disk and that library was not currently listed in the Available File-based Libraries, you would define the search as follows:
Select the Models option in the panel's upper libraries menu () in order to include library model collection entries in the Categories listing. The additional entries in this browsing mode include Symbol, Footprint and Simulation model collections sourced from the connected Workspace, and also installed PCB footprint libraries (
In the Available File-based Libraries dialog, Footprint Library files will be listed under the dialog's Project and Installed tab regardless of the Models view setting.
Within the component listing grid itself, the content that is included in the list is managed by:
Grouping the list by column data – right-click in a column header, select the Enable Columns Grouping option then drag a column header (e.g.,
Footprint) into the grouping space at the top of the list. The list entries will be collected under each unique parameter (e.g., type of footprint) from the specified grouping column.
There are various manners in which you may display the contents within the Components panel. When right-clicking on the names of each column (Name, Description, Footprint) you may select from the following options, depending on how you wish to display the components:
To search for available components in the Components panel, enter a phrase in the Search field and/or use the panel's Categories and Filters selections to narrow the component listing to your specific needs. Filters are supported for Workspace components only, and as in the Manufacturer Part Search panel, the Components panel supports unit-aware (text to number) search filters. The search functionality prioritizes results according to the entered search criteria.
The Search function allows you to select then edit or add to an active Search string. Click the 'active' search string to enter it into the Search field. You can reuse or edit that search from the Search field.
The Find Similar Components dialog provides the possibility to define search preferences based on the selected component.
The Find Similar Components dialog is used to define your search preferences based on the selected component. The final search results will depend on the selected component type, be it Workspace or non-Workspace components, and your Workspace connection status. For example, Workspace components will often display more parameters than a non-Workspace component. To specifically gather components and parameters that are the same or different from the one selected, the drop-downs may be utilized to select Same, Any, or Different choices.
The dialog can be accessed by right-clicking on a listed component, then selecting Find Similar Components.
A selected component is placed on a schematic by dragging and dropping, by selecting Place from its right-click context menu, by using the button in the Details pane, or by using the Enter hotkey.
When viewing Workspace components, the Filters pane is populated by selected filter options based on the current search and available parameters. Parametric filtering of the listed components provides further options for locating a specific component or type of component. Open the Filters pane from the button above the Categories pane.
Note that filters are only supported for Workspace components. Use the Filter Search field within the pane to find a specific parameter filter, and in the panel's narrow/docked mode, click the button to pop out the Filters as a panel extension.
The panel Filters options can be tailored to your needs by selecting particular parameter types as Favorites, which then shift to the top of the list for the current component Category. Hover to the right of a parameter filter’s name and click the icon to set the filter as a Favorite. Favorite filter settings apply to and are saved for individual component Categories.
To reset your favorites to the five default parameters, right-click then choose Reset Favorite Parameters.
For Workspace components, the right-click menu offers options to edit the component through the Single Component Editor (Edit) and perform component management functions such as component creation and cloning, or editing the selected component's Part Choices and Type (Operations).
Additional information options in the component Details pane include: viewing a model image, viewing online datasheets (References), live Supplier information (Part Choices), seeing where the part has been used in Workspace projects and Managed Sheets (Where Used), and through the right-click menu, the ability to copy selected or all component parameter data (technical details) in a tab-delimited format, and resetting favorites.
When browsing the components in a connected Altium 365 Workspace and if any issues regarding the health of the selected component are found, an indication of it will be presented by the (for errors) or (for fatal errors) icon in the Component issues line above the component parameter list. The number at the right of the icon indicates the number of found issues. Click the down arrow at the right of the number to see the short descriptions of the issues.
You may use the custom filtering feature to further refine filtering in the Components panel. The feature is available by clicking the filter () icon in the header, then selecting
(Custom). This will open the Filter Editor dialog, which allows you to define the condition, operator, value, operator type, etc., for which you want to filter results.
The Where Used drop-down tracks where a particular component is located. You may select the Project, Managed Sheets, or All buttons to view the particular project, managed sheet, or both, in which the given component has been used. Information regarding the date and time of placement is available, as well as information regarding the soft delete feature, in the case that the component has been deleted.
Operating as a 'soft delete', the removal process provides increased options and information as you proceed, including relevant links to source items for review purposes. Items can be deleted by users who have editing rights to those items and can be restored from within the Workspace's browser interface. In the Workspace, deleted items are moved to a dedicated Trash location where they can be retrieved (Restore) by users who have editing rights to the deleted items, or completely removed (Permanently Delete) by Workspace administrators or the owner of those items.
When using the Components panel, the data for Workspace components are cached to the local machine from the Workspace. This provides an offline access mode for Workspace components when Altium Designer is not connected to the Workspace, and therefore allows normal component browsing and placement, etc. Note that Filters are not enabled in this mode.
This condition is indicated by the 'Offline mode – cached data is being used' warning text in the lower bar of the panel’s component list pane. The cache builds up component data over time and may be cleared (for all Workspaces) using the Clear Cache option that is available under Known Servers in the Data Management – Servers page of the Preferences dialog.
Edit the Part Choices List associated with a Workspace component by selecting the Operations » Create/Edit PCL option from the entry’s right-click menu.
Use the following Edit Part Choices dialog’s button to open the Add Part Choices dialog, which will automatically search for part manufacturers by the selected component's
Name parameter. Deselect the predefined search term to manually search for alternatives – functionally, the dialog is a modal version of the Manufacturer Part Search panel.
Part Choice entries in the list can be ranked by selecting an appropriate star icon level, where the list will automatically be reordered with the highest-ranked manufacturer choice at the top.
A Part Choices List is carried with the component wherever its data is applied, such as in a Schematic design, BOM document, Output Report, and so on.
The right-click pop-up menu for the panel provides the following commands:
The Compare feature allows you to compare the parameters of two selected parts. This feature is accessed by selecting two components (parts) in the grid region with the icon enabled (blue). The Selected Component Details region opens to the right of the grid region. The upper region (region 1 in the image below) displays an image, the name, description, and price of the selected parts side-by-side. Click the Datasheet button to open the manufacturer's datasheet (if available) for the associated component. Click the Place button to place the component in the design space. The component will appear floating in the design space; click to place the component in the desired location. You can continue to place additional components or right-click or Esc to leave placement mode and return to the Components panel.
The lower region (region 2 in the image below) displays a side-by-side view of the components' parameters, with differences highlighted in red text for easy comparison.
The Compare feature is also available when the Components panel is in compact mode, though works a tad differently. This feature is accessed by selecting two components (parts) in the grid region. The Selected Component Details region opens below the grid region. The upper region displays the name, price, and view of the components' parameters, with differences highlighted in red text for easy comparison. The lower region displays a side-by-side view of the components' Symbols and Models.
The symbol and footprint of a given component can be hidden within the Models section of the Details pane, which is accessed by clicking on the upper right. Once hidden, the symbol and footprint will be replaced with clickable links that revert the hidden items to their original view. Also included is the ability to scale the size of the displayed models. For both the symbols and footprints, click and drag the lower perimeter of the model area to resize the image.
For a Schematic Library (
.SchLib) file being browsed in the Components panel, the symbol and footprint of the selected component can be edited using the button at the bottom-right of the model preview.
The ability to edit a footprint is made available when accessing the Components, as long as valid and linked footprints are already present.
The search engine and view used in the Components panel is also applied in other Altium Designer applications where a component choice is made. The component search functionality is included in these (modal) dialogs, along with an OK confirmation button and minor variations in the available action commands. The dialog is typically called Component Search.