Component Management in CircuitMaker
Parent page: Exploring 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.
Watch a short video about CircuitMaker Components. Note: This video applies to a previous release of CircuitMaker.
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 CircuitMaker Community Vault components, if available.
The CircuitMaker Community Vault is a cloud-based storage and management repository that hosts CircuitMaker component files. Each Vault 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 need to directly access the Octopart database or the Community Vault, 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.
To access the Octopart component listing for your design projects, open the Libraries panel from the main ribbon menu (View | System | Libraries) and ensure that the Octopart library (rather than Favorites or Projects) is selected in the top drop down menu. Note that the panel will pop out from the right side of the screen, but can pinned to remain open (), or undocked by dragging its title bar away from the side.
Use the Libraries panel search box () to narrow the Octopart listing to component types of interest. The majority of listed parts are linked to a CircuitMaker component and models in the Community Vault, indicated by the presence of the icon attached to the entry's preview image.
Hover the cursor over an entry to see a summary of the component's specifications.
Each entry in the panel's component listing is composed of, at a minimum, a link to its Octopart web page entry. Clicking on the link will open the component web page within CircuitMaker – this includes the HTML version of the available component data, including supplier pricing, specifications, data sheets, etc.
Components entry's that have a CircuitMaker component available in the Community Vault will also include relevant data extracted from the Vault. This is arranged in the lower section of the Libraries panel, and includes the component model data and revision references.
To access further information about the CircuitMaker Vault entry for the selected component, right click the entry and choose Component Details from the context menu. This opens a dedicated page for that vault component which provides its full details, such as its Watch and Ratings settings, applied Tags, a list of its historical revisions, and an indication of any CircuitMaker projects that use this component version.
To use a component listed in the Libraries panel 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.
Note that components cannot be Placed on project documents that are designated as 'Read Only' – such as those in another CircuitMaker user's project – but can be placed on a new revision (version) of that document.
Build a Listed Component
If a Community Vault 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 Vault for others to share. CircuitMaker provides component editors for defining a component's parametric information and models, for all design domains (schematic, PCB and Simulation).
While a CircuitMaker component can, for convenience, be considered as a single package of data and models in the Community Vault, these elements are in fact separate. The vault component entity (or 'item') is composed of just the base ID and parametric information, and the models are separate vault items that are linked to the component item.
A vault component is therefore built up from a master Component item (with its own editor in CircuitMaker) plus a number of linked types of Model items (each with their own editors in CircuitMaker).
To create a component that will be linked to the currently selected entry in the Libraries panel list, click the button or right click the entry and select Build This Component from the associated context menu.
This will open a new vault component entry in CircuitMaker's component editor, which is prepopulated with the component information (Comment, Description and Parameters) provided by the Octopart component database.
The new CircuitMaker component is ultimately composed of the component's parametric information – that 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 (Committed) to the Community Vault.
Note that all data entries can be changed in the editor, but any edits to Comment and Description fields will be exclusive to the new vault component. That is, they will not show in the Libraries panel component list, as this information is defined by the Octopart component database source.
Add a Symbol
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.
To add a basic schematic symbol to the new component, click the Home | Symbol button on the main ribbon menu and choose an appropriate graphic symbol. The selected symbol will open in CircuitMaker's symbol editor for further editing.
Alternatively, you can you use a Symbol that has already been created by selecting Use Existing Symbol. This opens a symbol browser dialog allowing you to view and select from a list of existing schematic symbols, then edit and save a new version for your component.
Alternatively, to create a new, custom schematic symbol for the new component, click Create new symbol (above) or use the Click to add new symbol link in the component editor Models section:
CircuitMaker's symbol editor will open, where the new schematic symbol can be formed using the tools available under the Home tab on the main ribbon menu.
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 Schematic Symbol Properties dialog by selecting Home | Library » Component Properties from the ribbon menu. Use the dialog to define properties such as the component's Comment attribute or default Designator, or to add custom Parameters, and so on.
When complete, save the new symbol from the main menu (File » Save) or by right clicking on the symbol file in the Projects panel and selecting Save from the context menu.
Add a Footprint
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.
To add a footprint in the component editor, click the Home | Footprint button on the main ribbon menu and choose Create new footprint or Use existing footprint. In the same way as using an existing component symbol (see above) the Use Existing footprint options opens a browser dialog that allows you to view and select from a list of existing footprints, then edit and save a new version for your component.
To create a new, custom footprint for the new component, select the Create new footprint option or use the Click to add new footprint link in the component editor Models section:
CircuitMaker's footprint editor will open, where the new footprint can be formed using the tools available under the Home tab on the main ribbon menu.
Footprints are created by placing pads, tracks, lines, arcs, 3D elements, 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 Component properties dialog by selecting Home | Library » Component Properties from the ribbon menu. Use the dialog to define properties such as the footprint's description, etc.
When the footprint design complete, save the new footprint from the main menu (File » Save) or by right clicking on the footprint file in the Projects panel and selecting Save from the context menu.
Note that the Projects panel shows (temporary) documents for the Component (CMP-xxx) and its sub models – in this case, a Schematic Symbol (SYM-xxx) and the PCB Footprint (PCB-xxx). A Simulation model will appear as a SIM-xxx document.
Add a Simulation Model
A Simulation model provides the necessary component simulation data for circuit analysis by a Spice Simulation engine. When a valid Simulation model is associated with a CircuitMaker component, it becomes simulation ready when placed in a schematic design document.
To add a Simulation model in the component editor, click the Home | SIM Model button on the main ribbon menu and choose Create new simulation or Use existing simulation, where the latter opens a SIM Model browser dialog allowing you to view and select from a list of existing simulation models, then edit and save a new version for your component.
To create a new, custom SIM model for the new component, select the Create new simulation option or use the Click to add new simulation link in the component editor Models section:
CircuitMaker's simulation editor will open, where the new simulation data can be added and configured within the main editor page. When the simulation model data is complete, save the new SIM model from the main menu (File » Save) or by right clicking on the simulation file (SIM-xxx) in the Projects panel and selecting Save from the context menu.
Commit to Vault
Returning to the main component editor you can now see that both a Symbol and Footprint model (shown as previews) are associated with new component. When the component is saved (Committed) to the Community Vault, links from the base component to its models (which are also saved to the vault, automatically) are retained.
To save the new component (and its models) to the Vault, click the Home | Commit button on the ribbon menu.
This will instigate CircuitMaker's automated Commit process, which transfers (releases) the component and model file data to the Community Vault, configures the new vault component and adds access links in the CircuitMaker's Favorites Library.
The newly built component now becomes available to all CircuitMaker users through the Community Vault. The component 'version' you have built is a unique vault item that cannot be overwritten by other users. When another user edits this component, a new version (and vault item) is created - see Edit a Component, below.
If you do not wish to Commit the new component (or an edited component) to the Vault, click the Home | Discard changes button. This will remove the local component and model documents (CMP, SYM, PCB, etc) and close all editors.
Edit a 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 Vault (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 to delete a model.
When the component edits have been saved and then committed to the Vault, you may notice that the Component's alpha-numeric code has incremented – in the above example, CMP-1248485-1 will now appear as CMP-1248485-2 when selected in the Libraries panel (Octopart) list. This is because the edited component has been stored as a new version in the Vault, leaving the previous version (1) intact.
This represents the Community Vault's version control system at work. In short, when a component or model is committed to the vault, the version control system creates a new version – or more correctly, revision – of that component/model.
Build a New Component Version
In contrast to simply editing an existing component and its models, a new version of that component can be created using the Build New Version option, available from the right click menu of a component selected in the Libraries panel – or by simply clicking the button for a component that has a CircuitMaker component in the Vault.
While similar to the Edit process outlined above, it actually creates a new version of the selected component, prior to being committed – in terms of the initial component build outlined above (revision 1), the new component version would be revision 2. Models can then be added to the component in the normal way, to create an updated version of the selected component.
Note that the Edit process also creates a new version/revision when committed, so the practical difference here is that the new component version effectively reverts to its base state, with no models etc.
Build 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.
Note that a custom built component will not offer all the benefits of a component derived from the Octopart database, such as direct access to pricing, stock information, datasheets and so on.
To create a new custom component, select the Build your own option from bottom area of the Libraries panel.
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 Vault.
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 vault-based 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 Library from the context menu. Note that this option is only available for component entries that have an associated Community Vault component.
The Favorites component list is directly accessible from the Libraries panel by selecting Favorites in the panel's library selection drop down menu.
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 and also Tagged to provide filtered group listings – see the right-click context menu for these commands, and also the Remove From Favorites Library command.
When a component has been added to the Favorites list – either automatically or by manual addition (right-click » Add to Favorites Library) – refresh the listing by right clicking in the list and selecting Refresh Library from the context menu.
In the Favorites listing mode, the panel's component entries can also show a range of additional information, which is configured by right-clicking on an entry and choosing Select Columns from the context menu.
In the Select Parameter Columns dialog, select a desired parameter column on the left then it to the enabled list, or a displayed parameter column from the list on the right. Perhaps the most useful additional entry is the component RevisionID parameter, which will indicate the Revision state of each entry (see below).
One fundamental difference with the Favorites list, compared to the normal Octopart listing, is that its entries refer directly to Vault-based components rather than components in the Octopart database list. Each entry therefore includes information derived from the vault component item, such as its version – Revision ID (1, 2, etc).
As you can see from the above image of the Libraries panel, the Favorites list can include multiple entries for one component – note the 'ON Semiconductor LM317…' entries. Here, the two LM317 entries represent two versions of the vault component; the initial 1 revision and the 2 revision created by a subsequent edit – these were automatically added to the list during the Commit process.
Conversely, the other listed entries shown (components created by other users) have been manually added to Favorites from the Octopart library listing. Note that the entry highlighted in gray is at revision 4, which was the current version of that component when it was added to the Favorites list.
The Community Vault component associated with an Octopart component list entry will be the latest version of that vault component. If this is added to your Favorites list, the entry will stay at that revision, even though subsequent revisions may have been created by another user.
Note that the Octopart listing in the Libraries panel will always link to the current version (most recent revision) of a vault component.
To assist in collating and finding components in the Libraries panel Favorites list, component Tags are available to group component entries together.
When tags have been applied to individual component entries, the Favorites listing can be filtered to include just those components with a specific tag applied. To apply tags to a selected component entry, right click and select Tags from the context menu to open the Tags Editor dialog.
Tags need to be created before they are applied to a component. Click the dialog's button to create a new tag entry for the Available Tags list, and then apply one or more tags to the currently selected component using the button.
With suitable tags applied to the Libraries panel Favorites entries, the listing can be filtered by selecting one or more tags options from the panel's Tags drop down box – click the button at the right of the library selector menu. Check the box of each tag that will apply to the filter and wait for the list to refresh. Multiple tags imply a boolean OR relationship – if a component has any one of the checked tags, it will be listed.
The Favorites list will now only include those component entries that match the selected tag criteria.
Along with the Favorites entries listed in the Libraries panel, the entries are also available in the Favorites Library section of CircuitMaker's Start page – select View | Start or Home | Start from the main ribbon menu.
Entries on this list can be selected to open a dedicate page for that vault component. This 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 Vault component itself, including previews of its models (symbol, footprint, etc), Watch and Ratings settings, applied Tags, a list of its historical revisions, and an indication of any CircuitMaker projects that use this component version.
Revisions and Ratings
A Favorites Library vault component page provides access to that component's full set of Revisions – all versions that have been built for that component. A component page will always open to show the most recent revision, but a previous revision can be opened by clicking on its entry in the Revisions list.
This allows you to compare revisions of the current component and then Rate your preferred version. To rate the currently open revision, click on the star rating graphic to open its dialog, include an optional comment and select a rating level. Note that you cannot rate component revisions that you have created.
When viewing a component in the Favorites Library, the rating level for each component revision is shown in the Revisions list, where it also determines its position in the list order – the list is ordered by descending rating.
The overall rating for a component revision is computed as an average of all ratings applied by CircuitMaker users. In this way, the version of a component (revision) that most meets the approval of the CircuitMaker community will be rated highly, and will 'float' to the top of the component Revisions list.
Within a Favorites Library component page, any revision of that component can be Edited to create a new revision.
With the desired revision active (as loaded from the Revisions list) click the button to open that revision in the CircuitMaker component editor. The process of editing the component revision will create a new version of the component in the vault when the edit has been committed. In the case of the LM317MSTT3G component shown above for example, editing an available revision (1 or 2) would create a new revision 3.
When a Watched component is edited, or more accurately, if a new version is created, an automated alert email will be sent to your registered CircuitMaker email address. The Watch function is automatically enabled for a component that you have created or edited.
Project Library mode
To provide direct access to the components used in a CircuitMaker project, the Libraries panel offers an additional library list mode – Project. When this mode is selected, the Libraries panel list is populated with the components used in the currently loaded (and selected) project.
Switch to the Projects component list mode by choosing Project from the panel's top drop down menu.
Components entries are added to the Project library as new parts are added to the current project.
As with the other Library panel list modes, components may be edited (to create a new revision), added to your Favorites library or opened to the detailed view page. Note that components cannot be Placed in project documents that are 'Read Only' – such as another CircuitMaker user's project – but can be placed in a new revision of that document.