A Guide to Component Management in CircuitMaker

A component is the general name given to a part that can be placed into an electronic design during the design capture process. In its common form, a component is generally composed of a logical symbol that is applied to the design’s schematic, and a footprint pattern (model) that will physically represent the component on the PCB.

Components are collected together in Component Libraries where they can be extracted and placed in a design document, such as a schematic layout, and then ‘wired’ together to form the complete design.

CircuitMaker Components

In CircuitMaker, components are accessed from the Libraries panel – the central point for locating, reviewing, using and creating CircuitMaker components. This presents a searchable list of components sourced through the Octopart component database portal, which provides access to comprehensive component data for thousands of real-world components. In the background, the components listed in the Libraries panel are linked to matching components in the cloud-based CircuitMaker storage and management repository (community components), if available. Each community component is effectively a 'package' that contains the data and models (symbol, footprint, etc.) that make up a complete CircuitMaker component, which is linked to a matching Octopart component entry in the Libraries panel.

When using CircuitMaker, there's no direct access to the Octopart database or the CircuitMaker repository, as all data sourcing and linking is performed in the background. Your central access point for CircuitMaker's automated component management system is the Libraries panel.

Libraries Panel

Panel page: Libraries panel

To access the component listing for your design projects, open the Libraries panel from the main ribbon menu (View | System | Libraries) and ensure that the All Parts entry (or a sub-category of it) is selected in the top drop-down menu. Note that the panel will pop out from the right side of the screen, but can be pinned to remain open (), or undocked by dragging its title bar away from the side.

Each entry in the panel's component listing is composed of, at a minimum, a link to its page on the manufacturer's website. Use the selection options in the categories drop-down menu () and the Search field to narrow the listing to component types of interest.

Use the panel's category drop-down and search capability to narrow the listing to component types of interest.

Many of the listed parts are linked to a CircuitMaker component and models in the community library, indicated by the presence of the icon in the list. Using the panel's filtering capability, you can show only those components that have models – click the  icon in the model column header and check Yes.

The component listing can be filtered to show only components with models.

To use a component equipped with a model in your design, simply drag it on to an open schematic design document, click the button, or right-click the entry and select Place from the context menu.

A component can be placed from the Libraries panel to your design.

Along with the component entries listed in the Libraries panel, community components are also available on the All Components tab of the workspace.circuitmaker.com website's Components page. You can use the component search box to search for a specific component. Entries on this list can be selected to open a dedicated page for that community component.

Community components can be inspected on workspace.circuitmaker.com.

A community component's page provides the full details of the component derived from the Octopart component database data, including its specifications, supplier options, stock levels, and pricing information. The component page also includes data derived from the community component itself, including previews of its models, a list of its historical revisions, and an indication of any CircuitMaker projects that use this component revision.

An individual component page which provides direct access to the community library data for that component.

Create a Listed Component

If a community component is not available for the component you have selected (the icon is not shown), it can be created within CircuitMaker and automatically added to the community library for others to share. CircuitMaker provides the Component Editor for defining a component's parametric information as well as Schematic Library and PCB Footprint Library editors for defining schematic and PCB domain models respectively.

To create a component that will be linked to the currently selected entry in the Libraries panel list, right-click the entry and select Create New Component from the associated context menu. This will open a new community component entry in CircuitMaker's Component Editor, which is prepopulated with the component information (Comment, Description, and Parameters) provided by the Octopart component database.

If a component does not have models, you can create them by yourself.

The new CircuitMaker component is ultimately composed of the component's parametric information – that is shown on the initial screen – and any models you would like to add. At least one model needs to be added before the component can be saved to the community library.

Add a Model

A schematic symbol is a component's graphical object that represents the component when it is placed in a schematic document. The symbol includes electrical connection information (indicated by component pins) that allows a circuit to be logically wired together, and to be matched to its equivalent footprint connections (Pads, etc) in the PCB domain. A PCB footprint is a component's graphical object that represents its physical and connectivity form when it is placed in a PCB document. The footprint includes both electrical and mechanical connection information (primarily indicated by PCB pads) and allows the components to be interconnected by tracks in a board layout design.

You can use a model that has already been created by selecting Add Existing from the Home | Add New Symbol or Home | Add New Footprint button menu respectively or clicking the drop-down icon on the button below a model type in the Models section of the Component Editor and choosing Existing from the associated menu. This opens the Select Item Revision dialog allowing you to view and select from a list of existing models, then edit and save a new version for your component.

Add an existing model to the new component. Here is shown adding an existing schematic symbol to the component. Hover the cursor over the image to see adding an existing PCB footprint to the component.

Alternatively, to create a new, custom model for the new component, select the Home | Add New Symbol or Home | Add New Footprint button in the ribbon or click the drop-down icon on the button below a model type in the Models section of the Component Editor and choose New from the associated menu. The respective editor will open, where the new model can be formed using the tools available under the Home tab on the ribbon.

Symbols are created by placing shapes and applying the drawing tools, and importantly, by including connection Pins that define the component's electrical wiring points in a schematic document. To edit the schematic symbol's properties, open the Symbol mode of the Inspector panel by selecting Home | Library » Component Properties from the ribbon. Use the panel to define properties such as the component's Comment attribute or default Designator.

Footprints are created by placing pads, tracks, lines, arcs, 3D bodies, etc. on suitable PCB layers to accurately represent the physical and electrical attributes of the component in the PCB domain. To edit the footprint's properties, open the PCB Library Footprint dialog by selecting Home | Library » Footprint Properties from the ribbon. Use the dialog to define properties such as the footprint's description, etc.

Create a new component model using the relevant editor. Here is shown the Schematic Library editor. Hover the cursor over the image to see the PCB Footprint Library editor.

When complete, save the new model using the  icon in the Quick Access Bar (shortcut: Ctrl+S) from the main menu or by right-clicking on the model entry in the Projects panel and selecting Save from the context menu.

Save to Community Library

Returning to the Component Editor, you can now see that both symbol and footprint models (shown as previews) are associated with the new component. When the component is saved to the community library, links from the base component to its models (which are also saved to the library, automatically) are retained.

The Component Editor showing previews of its associated symbol and footprint models, prior to being saved to the community library as a 'full' component.

To save the new component (and its models) to the community library, click the Home | Save to Server button on the ribbon. This will instigate CircuitMaker's automated saving process, which transfers (releases) the component and model file data to the community library, configures the new community component, and adds access links in the CircuitMaker's Favorites list. The newly built component now becomes available to all CircuitMaker users through the community library.

If you do not wish to save the new component (or an edited component) to the community library, click the Home | Discard changes button. This will remove the local component and model documents and close all editors.

Save the component to the community library or discard changes to abort the process.

Edit a Community Component

If you want to make changes to an existing component and its models, select the component in the Libraries panel list and select Edit from the right-click menu. This will retrieve the component from the community library (or local cache) and open it in the Component Editor, as shown above. If you subsequently choose to edit one of the models (click the  icon), it will be retrieved and opened in its respective editor. Use the Remove command from the  icon menu to delete a model.

Create a Custom Component

There may be circumstances where a specific component that you need for a design is not listed in the Octopart database, and therefore not included in the available component list in the Libraries panel. This can be is resolved by creating a new, unlisted CircuitMaker component from scratch – a custom component.

To create a new custom component, select the Create Custom Part option below the component list in the Libraries panel or in the component list area when there are no components found.

If there are no relevant parts, you can create your own custom part.

This opens a new blank component entry in the Component Editor, which can be populated with the information that corresponds to your custom component. In the same way as building a new listed component (outlined above), models can then be created and the component committed to the community library.

Favorites Only Mode

Along with the Octopart component database listing available in the Libraries panel, CircuitMaker also offers the concept of a Favorite collection of components. These represent community components that you created or edited, or any that you have manually added to the Favorites list.

To manually add a component from the Octopart listing in the Libraries panel to your Favorites collection, right-click on the component entry and select Add To Favorites from the context menu. Note that this option is only available for component entries that have an associated community component.

A community component can also be added to your Favorites list from its component page on workspace.circuitmaker.com. To do this, use the  button on the page.

The Favorites component list is directly accessible from the Libraries panel by selecting Favorites Only in the panel's library selection drop-down menu.

The Favorites library setting lists and groups only the components that interest you.

Building up a list of favorite components means that your preferred component options are easy to access and use in your designs. Components can be placed in a design from the Favorites list using the Place button or right-click menu command and also removed from the list using the Remove From Favorites right-click menu command.

Using the Custom Only checkbox below the Search field, you can display in the panel only your Custom Components. Note that custom parts are distinguished by the  icon in the Favorites list.

As you can see from the above image of the Libraries panel, the Favorites list can include multiple entries for one component – note the 'LM217MS-TR' entries. These represent two versions of the community component; the initial revision 1 and the revision 2 created by a subsequent edit – these were automatically added to the list during the saving process.

Conversely, the other listed entries shown have been added to Favorites from the Octopart library listing. Note that the entry highlighted in blue is at revision 2, which was the current version of that component when it was added to the Favorites list.

Along with the Favorites entries listed in the Libraries panel, the entries are also available on the Favorites tab of workspace.circuitmaker.com website's Components page. Entries on this list can be selected to open a dedicated page for that community component.

The list of your favorite components can be viewed on workspace.circuitmaker.com.