Component Management in CircuitStudio

Parent page: Exploring CircuitStudio

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 ‘wired’ together to form the complete design.

The initial task in this part of the design process is generally capturing its circuitry in a schematic, where a placed component provides a graphical symbol that includes the component’s electrical connection points defined by pins. In CircuitStudio, this schematic representation of the component also provides a range of optional properties, parameters and links to a PCB footprint pattern – or more correctly, a 2D and/or 3D model that physically represents the component on a PCB.

Schematic component definitions (composed of a symbol, model links, parameters. etc.,) are collectively stored in a Schematic Library file (*.SchLib) that can be loaded in CircuitStudio. PCB model definitions are similarly stored in a PCB Library (*.PcbLib), where its constituent models are linked to by the symbol (component) definitions in a Schematic Library.

The base schematic component definition in a Schematic Library includes links to suitable PCB models in a PCB Library, satisfying both domains with a unified component.

This unified component format means that its schematic representation provides all the information required to implement a component in both the schematic and PCB design domains. When a schematic design is transferred to the PCB domain (through the Update PCB process), CircuitStudio will locate and place the PCB model(s) defined by the schematic component’s model link(s).

Working With Sch/Pcb Libraries

In CircuitStudio, individual schematic and PCB library files can be used in a several ways depending upon requirements:

• Library files can be added to a design project, where they will be available for use whenever the project is loaded.
• Libraries can be stored separately then installed in CircuitStudio as permanently available libraries.
• Schematic and PCB library files can be added to a Library Package project, which can be compiled to create a single Sch/Pcb Integrated Library file. See below for more information.

In all cases, the central point for accessing and installing Schematic and PCB libraries is via the Libraries panel – select View |System | Libraries. The panel provides a list of components (symbols/models) in the currently selected library, including a preview of each component entry’s symbol and/or footprint.

When viewing an opened schematic library, which contains the base information for a unified component, the Libraries panel displays a graphic summary of any linked PCB models.

The Libraries panel is command central for all common component and library management tasks.

Libraries can be added to the current project or installed through the Available Libraries dialog, accessed from the panel’s button. Libraries can also be installed in the Data Management – Installed Libraries page in CircuitStudio's Preferences dialog (File » ).

Editing Components

Components contained in individual schematic and PCB libraries can be edited (or created/deleted) with CircuitStudio’s library editor and the associated SCH/PCB Library panels.

To open a schematic component for editing, right-click its entry in the Libraries panel list then select Edit Component from the context menu. Similarly, to open a component for editing in an opened PCB Library, select Edit Component from the Libraries panel right-click context menu. Note that a library can also be opened for editing directly from the Projects panel.

The components contained in individual Schematic or PCB libraries can be edited down to the fundamental elements and primitives.

CircuitStudio will open the appropriate Library panel for the component type being edited (SCH Library panel or PCB Library panel) and load the symbol or model graphic in the editor workspace, ready for editing. The Library panel can be manually opened from the ribbon menu if necessary from the schematic library editor or PCB library editor: View | Schematic | Library or View | PCB Library | Library.

For component editing, the system provides a comprehensive set of graphic editing tools for both schematic symbol and PCB pattern editing (available from the Home menu tab), while the Library panel delivers higher-level editing functions such as adding/deleting component entries and accessing a component’s basic elements. For schematic symbols, these are the electrical pins, and for PCB patterns these are tracks, pads and 3D elements that make up the model.

Component Data and Linking

Beyond the inclusion of library-based symbols and patterns, a comprehensive, multi-domain component needs to contain additional information such as its base specifications, parameters and 2D/3D model links – the full descriptive data set for a unified component.

This data is stored in the schematic component itself and can be edited through the schematic Library Component Properties dialog. With the schematic library editor open, this can be accessed by selecting Home | Library | Library » Component Properties from the main menu, or by double-clicking on the component name entry in the SCH Library panel.

Along with a set of basic component properties, a component can have several linked models and any number of custom Parameters added.

Perhaps the most crucial aspect to the creation (and maintenance) of a unified component are the component Schematic-PCB model links. These are established and edited in the Models region of the Library Component Properties dialog. Here, 2D and 3D library models can be added, removed and edited from the section’s matching buttons and the associated PCB Model dialog (accessed by clicking Edit in the Library Component Properties dialog).

The base schematic component can be linked to a variety of model data.

The PCB Model dialog allows model links to be established from a loaded library, an absolute library path, a library in CircuitStudio's library search path, or by browsing the local system storage.

Integrated Component Libraries

The next evolutionary step in managing components in CircuitStudio is effectively bringing individual Schematic and PCB libraries together as single Integrated Libraries.

These compile all the required component elements (Schematic symbols, PCB models, etc.,) into a single read-only library file (*.IntLib). The components contained in an Integrated Library are persistently unified across the Schematic-PCB domains since the internal model links are permanent – that is, they cannot be broken, as is the case when component elements in separate Sch/PCB library files are linked.

PCB models are imported into an Integrated Library component when the library is created.

In practice, an Integrated Library behaves like a read-only Schematic Library that contains (rather than links to) PCB models for each component. The library type is, therefore, both secure and portable.

Examples of Integrated Libraries can be found in CircuitStudio’s local Library folder, C:\Users\Public\Documents\Altium\CS\Library, and the Miscellaneous Integrated Libraries are usually installed by default – Miscellaneous Connectors.IntLib and Miscellaneous Devices.IntLib.

Creating an Integrated Library

A CircuitStudio Integrated Library is produced from a specialized project type called a Library Package (*.LibPkg). In the simplest approach, an existing Schematic Library (with valid model links) is added to this project, which is then compiled to produce a separate Integrated Library.

The basic steps are:

• Create a Library Package project by opening a new Integrated Library project (File » New Library).
• Save the project as a suitable name (File » Save Library As).
• Add a target schematic library to the project (Project| Design Documents | Add Existing Document).
• Compile the project to create the matching Integrated Library (select the package project name then choose Compile Integrated Library xx.LibPkg from the right-click context menu).
• Check for a successful compile result as indicated in the Messages panel (View | System | Messages).

A Schematic Library has been added to the MyIntLib Library Package project and compiled to create the MyIntLib Integrated Library.

Note that the Integrated Library generated by the process (saved in ../Library/Project Outputs for xx) is automatically installed in CircuitStudio, ready for use. The self-contained library file, which includes the component symbols parameters and PCB models, can be safely transferred to storage or other users as part of a project or as a free standing library.

The new Integrated Library (MyIntLib) installed in CircuitStudio.

Altium Vault Components

The most sophisticated and comprehensive solution to managing components in CircuitStudio is making use of the Altium Component Vault – a separate, fully managed repository of up-to-date components provided by Altium.

Along with providing a huge range of components available for use in your designs, the cloud-based vault content is managed by Altium in partnership with major parts suppliers. This frees you from the task of managing component resources, since all parts are fully ratified, lifecycle is managed, and also offers a wide range of additional data such as current specifications, data sheets and pricing.

In practice, vault components are used in CircuitStudio by connecting the remote Altium Component Vault, browsing or searching for the desired part in the Vault Explorer, and placing it into the schematic design.

The CircuitStudio Vault Explorer provides direct access to components in the Altium Component Vault.

Component Supplier Links

While access to high quality component resources is essential to the success of a design, the symbols and models only represent the virtual equivalent of ‘real-world’ components – that is, the physical parts that are ultimately loaded into a manufactured circuit board. Deciding which actual parts are used in the design – with what specifications, from which manufacturers and suppliers, and at what price – is a crucial part of the design process that usually involves considerable research and product comparison.

CircuitStudio relieves this process while greatly improving its accuracy and relevance through the provision of Live Supplier Links. Easy and quick to implement, these are live links established between a CircuitStudio component and an item in a supplier's database of electronic components.

The Supplier Link is formed by a direct connection to supplier web services, which allows you to search across all supplier databases supported by CircuitStudio. When the desired part is selected, a link is added to the local schematic component as a set of parameters – Supplier and Supplier Part Number. This link connection is then re-established each time the component is opened in a schematic or library, and is, therefore, guaranteed to reflect the current supplier’s data for that component.

In an existing schematic design, a component’s Supplier Links can be seen through its Properties dialog (double-click on a schematic component).

A component's Supplier Links are held as parameters in the schematic component entry as supplier and part number fields.

To see the data that a component’s Supplier Link extracts from the supplier’s web services, right-click the schematic component then select Supplier Links from the associated context menu. Note that Supplier Links can be both added and removed from this dialog.

The Supplier Links dialog displays any supplier links attached to the selected component and the resulting data extracted from associated supplier web services.

Being able to establish supplier-linked component data early in the design cycle, and review this information throughout the design process, allows you to make valid part decisions based on current component specifications, data sheets, physical properties, and availability and pricing information. Additionally, once live Supplier Links have been added to CircuitStudio components, the linked supplier data – including pricing and stock information – can be included at design release time in a Bill Of Materials (BOM).

In CircuitStudio, Supplier Links can be added to components in a project or components within a Schematic Library. Supplier Links added to components in a project are exclusive to that project, and Supplier Links added to a library component will become available in any project that uses that library component.

Adding Supplier Links to a Project

To add Supplier Links to a component in a project, select the component in the schematic, select Supplier Links from the right-click context menu then click the Add button in the resulting Supplier Links dialog. The Add Supplier Links dialog opens. The dialog’s Keywords field will be pre-populated with the Comment property text for that component, which will be the nominal search string applied to the supplier databases when you select the Search button. Note that the keyword string is editable.

When the search results have populated, you can browse through the available options to determine the optimal part selection for the project component.

When adding a supplier link to a component, the Add Supplier Links dialog shows the full list of extracted supplier entries that match the dialog's keyword search.

When OK is clicked, the selected supplier part information will be added to the Supplier Links dialog, and when OK is clicked in the Supplier Links dialog, the selected supplier part information is added to the current component. An existing supplier link can be removed from the Supplier Links dialog list by selecting the supplier link to be removed then clicking the Remove button.

The supplier/part data is stored as the Supplier 1 and Supplier Part Number 1 parameters, as mentioned above. Note that multiple part links can be added to the Supplier Links dialog list. These will be stored as successively numbered Supplier parameters in the component – i.e. Supplier 1, Supplier 2, etc.

To see the resulting Supplier Link data in the project BOM, select Project | Project Actions | Generate outputs to open the Generate output files dialog. The BOM can be both previewed and configured by selecting the Configure link associated with the Bill of Materials in the Outputers region of the dialog. Note that different levels of supplier information can be included to the BOM by enabling and disabling data columns.

The BOM configuration dialog provides export and currency options plus a preview of the BOM contents.

Adding Supplier Links to a Library

Supplier Links are added to library components within the schematic Library Editor, instigated by opening a Schematic Library.

With the selected part opened in the editor, right-click within the workspace then select Supplier Links from the context menu. The part choices can be viewed and added from the Supplier Links dialog, as described above for adding links to a project.

Supplier Links added to a library component are stored with the component and are retrieved whenever that component is placed in a design from the library.

Where a library component has included Supplier Links, the Libraries panel will display current pricing information for that component, sourced directly from the primary supplier – the Supplier 1 parameter for that component. This provides a convenient view of the component's current pricing information, sourced from the live supplier link, whenever that component is selected in the library for potential placement in a design.

Live pricing data is available when a library component (that has embedded supplier links) is selected in the Libraries panel.

Supplier Choices

Through agreements with range of component suppliers, Altium has enabled CircuitStudio to access and search for component data from multiple sources. The web access to these supplier portals is provided by CircuitStudio Extensions – plug-in software modules developed to interface with specific supplier database APIs.

From the practical perspective, a supplier Extension needs be installed and active for the Add Supplier Link dialog to load and display that supplier’s data, and to also re-access the linked data from a project or library component.

The desired supplier options also need to be enabled, which is configured through the Data Management – Suppliers page of the Data Management section in the Preferences dialog. This also provides configuration options for defining your country or region, supplier login credentials (if applicable), import options, and search keywords.

See the Data Management - Suppliers Preferences page for more information of configuring suppliers and supplier data.