Parent page: Workspace Content Types
From a designer's perspective, a Workspace component gathers together all information needed to represent that component across all design domains, within a single entity. It could therefore be thought of as a container in this respect – a 'bucket' into which all domain models and parametric information is stored. In terms of its representation in the various domains, a component doesn't contain the domain models themselves, but rather links to these models. These links are specified when defining the component.
Altium Designer, in conjunction with your connected Workspace, caters for the ability to create and manage symbols (Symbol Items) in that Workspace. Such symbols are created directly within the Workspace. Once a symbol has been created (and data saved into a revision of it), it can be reused in the creation of one or more components.
Folder Type
When creating the folder in which to store symbols, you can specify the folder's type. This has no bearing on the content of the folder – saving a schematic symbol will always result in a corresponding Symbol Item. It simply provides a visual 'clue' as to what is stored in a folder and can be beneficial when browsing a Workspace for particular content. To nominate a folder's use as a container for symbols, set its Folder Type as Symbols, when defining the folder properties in the Edit Folder dialog.
Specifying the folder type – its intended use – gives a visual indication of the content of that folder when browsing the Workspace.
Item Naming Scheme
Another important aspect of the parent folder is the Item Naming Scheme employed for it. This defines the format of the unique ID for each Item created in that particular folder. Several default example schemes are available, utilizing the short-form code for either the folder type (SSL – Schematic Symbol Libraries) or the content type (SYM – Symbol):
$CONTENT_TYPE_CODE-001-{0000} – for example, SYM-001-0001.$CONTENT_TYPE_CODE-001-{A00} – for example, SYM-001-A01.$FOLDER_TYPE_CODE-001-{0000} – for example, SSL-001-0001.$FOLDER_TYPE_CODE-001-{A000} – for example, SSL-001-A001.
Using a default naming scheme, the software will automatically assign the next available unique ID, based on that scheme, having scanned the entire Workspace and identifiers of existing content. This can be a great time-saver when manually creating symbols.
A custom scheme can also be defined for a folder by typing it within the field, ensuring that the variable portion is enclosed in curly braces (e.g. SYMBOL-001-{0000}).
The Item Naming Scheme of the parent folder is applied to the Unique ID for each Item created within that folder.
The Item Naming Scheme employed for the parent folder can be changed at any time. The modified scheme will then be applied to any subsequent newly-created content within that folder.
Content Type
When creating a target Symbol Item in which to store your schematic symbol, ensure that its Content Type is set to Symbol, in the Create New Item dialog. If you are creating the Item in a Symbols type folder, this content type will be available from the right-click context menu when creating the Item.
Creating a symbol within a Symbols folder – the correct Content Type is available on the context menu.
Item Lifecycle Definition and Revision Naming
When defining a symbol, be sure to specify the type of lifecycle management to be used for the symbol, and the naming scheme employed for its revisions, respectively.
Control over which content types can use a particular lifecycle definition or revision naming scheme, can be defined and enabled at a global level from within the Content Types dialog, when defining each schema. The default schemes assigned for use by a symbol are: Generic Lifecycle and 1-Level Revision Scheme, respectively.
Once a schematic symbol has been saved into the initial revision of a Symbol Item, these schemes cannot be changed for that particular Item.
Specify the required schemes in the Create New Item dialog, using the Lifecycle Definition and Revision Naming Scheme fields respectively.
If the option to control use of lifecycle definitions and revision naming schemes per content type is enabled for any definitions/schemes, and the Symbol content type is not set to use a particular definition/scheme, then that definition/scheme will not be available in the applicable drop-down list.
Selecting the Lifecycle Definition and Revision Naming schemes for a manually created symbol.
Observing standard revision naming schemes and lifecycle definitions, across the various types of design content in a Workspace ensures smooth, consistent management of this content.
It is a good idea to add a Name and Description as part of the symbol's definition. This information is used when searching the Workspace and enables quick identification of what a symbol offers.
Saving a Schematic Symbol
Related page: Creating and Editing Content Directly through a Workspace
So far, we've discussed the support for a symbol in the Workspace, in terms of related folder and content types. Saving an actual defined schematic symbol into a revision of a Symbol Item can be performed in a streamlined way.
A schematic symbol can be edited and saved into the initial revision of a newly-created Symbol Item, courtesy of the Workspace's support for direct editing. Direct editing frees you from the shackles of separate version-controlled source data. You can simply edit a supported content type using a temporary editor loaded with the latest source direct from the Workspace itself. And once editing is complete, the entity is saved (or re-saved) into a subsequent planned revision of its parent Item, and the temporary editor closed. There are no files on your hard drive, no questioning whether you are working with the correct or latest source, and no having to maintain separate version control software. The Workspace handles it all, with great integrity and in a manner that greatly expedites changes to your data.
When you create a Symbol Item, you have the option to edit and save a schematic symbol into the initial revision of that Item, after creation. To do so, enable the Open for editing after creation option, at the bottom of the Create New Item dialog (which is enabled by default). The Item will be created and the temporary Schematic Library Editor will open, presenting a .SchLib document as the active document in the main design window. This document will be named according to the Item-Revision, in the format: <Item><Revision>.SchLib (e.g. SYM-001-0001-1.SchLib).
Example of editing the initial revision of a symbol, directly from the Workspace – the temporary Schematic Library Editor provides the document with which to define your schematic symbol.
Use the document to define the schematic symbol as required. For more information on doing this, see Creating a Schematic Symbol.
One important thing to observe is that only the symbol graphics need be defined – the representation of the higher-level component within the schematic editing domain. It is not a 'schematic component' as defined for use in older file-based component management methodologies, where other models and parameters are defined as part of that schematic component. A component needs only the graphical depiction of the symbol. It will include links to other domain models and parameters as part of its own definition.
There are three relevant controls when direct editing, readily available from the Quick Access Bar (at the top-left of the main application window), or from the Sch Lib Standard toolbar:
-
– Save Active Document. Use this button to locally save any changes made to the document. This allows you to save current changes, should you wish to come back at a later stage to make further changes before ultimately saving to the Workspace.
-
/
– Save to Workspace. Use this button to save the defined schematic symbol to the Workspace, storing it within the initial (planned) revision of the target Symbol Item. The Edit Revision dialog will appear, in which you can change Name, Description, and add release notes as required. The document and editor will close after the save. The library document containing the source schematic symbol, *.SchLib, will be stored in the revision of the Item.
A
Save to Server control is also conveniently provided to the right of the symbol's entry, within the
Projects panel itself.
-
/
– Discard Local Changes. Use this button if you wish to cancel editing and discard any changes made. The document and editor will close, and nothing will be saved to the target Symbol Item.
These controls are also available as commands – Save (shortcut: Ctrl+S), Save to Server (shortcut: Ctrl+Alt+S), and Discard Local Changes – from the main File menu and from the right-click menu of the symbol's entry in the Projects panel.
The saved data stored in the Workspace consists of the source schematic symbol, saved in a Schematic Library file named using the Symbol Item's Name. In the Explorer panel, switch to the Preview aspect view tab to see the symbol graphics.
Browse the saved revision of the symbol, back in the Explorer panel. Switch to the Preview aspect view tab to see the symbol graphics.
Reusing a Symbol
Related pages: Component, Controlling Access to Workspace Content
Once a schematic symbol has been saved to a Workspace, and its lifecycle state set to a level that the organization views as ready for use at the design level, that symbol can be reused in the creation of one or more components. When directly editing a revision of a component from a Workspace, how a symbol revision is added for use, depends on which mode of editing is being used:
-
Single Component Editing – the symbol revision is added to the component's Models region. Use the drop-down associated with the Add Symbol entry to choose the Existing command. An explorer-like dialog will open, with which to browse to, and choose, the required symbol revision.
Example of referencing a symbol revision as a model link, when direct editing a revision of a component using the Component Editor in its Single Component Editing mode.
You can edit a symbol revision directly from the
Models region by clicking the
button, at the top-right of the symbol preview.
-
Batch Component Editing – the symbol revision is added to the component's Model Links region. This region can be thought of in terms of a 'bucket' of domain models that can be accessed by any component definition. Assignment is a case of specifying which links are required for each definition. Click the Add control beneath the region and choose the SCHLIB entry. The Choose Models dialog will open (essentially an incarnation of the Explorer panel) with which to browse to, and choose, the required symbol revision.
Example of referencing a symbol revision as a model link, when direct editing a revision of a component using the Component Editor in its Batch Component Editing mode.
You can edit a symbol revision directly from the Model Links region by right-clicking and choosing the Edit command from the context menu.
Re-Saving a Symbol
At any stage, you can come back to any revision of a symbol in the Workspace, and edit it directly:
- From the Explorer panel – right-click on the revision and choose the Edit command from the context menu.
- From the Components panel – select the Symbols category (the Models option must be enabled in the panel's
menu for accessing this category), right-click on the entry for a symbol and choose the Edit command from the context menu.
Once again, the temporary editor will open, with the library (containing the source schematic symbol) contained in the revision, opened for editing. Make changes as required, then save the document into the next revision of the symbol.
Right-clicking on the top-level entry for a symbol itself, in the Explorer panel, or right-clicking on the symbol entry in the Components panel will edit the latest revision of that symbol.
Accessing the command to launch direct editing of an existing symbol revision from within the Explorer panel.
You can also update the revision of a symbol being used by a revision of a component directly on-the-fly, as part of editing that revision of that component. If the Component Editor is in
Single Component Editing mode, edit a symbol revision directly from the
Models region of the editor by clicking the
button, at the top-right of the symbol preview. If the Component Editor is in
Batch Component Editing mode, edit a symbol revision directly from the
Model Links region by right-clicking and choosing the
Edit command from the context menu.
Updating Related Components
When you make a change to a domain model – be it a symbol, footprint model, or simulation model – the moment you save that change into a new revision of the model, any components that use that model will become effectively out of date, still using the previous revision. In most cases, you will no doubt want to re-save those components, with the respective model links updated to use the latest revisions available. To streamline this process, a Workspace, in conjunction with Altium Designer, facilitates the ability to update related components – at the point of re-saving a model – after having made any modifications to that model through the direct editing feature.
The option to perform this update to the parent components can be found in the Create Revision dialog, that appears when saving the modified symbol back to the target Workspace. This option – Update items related to <ModelItemRevision> – is enabled by default.
<ModelItemRevision> is the current revision of the model, that is, the revision currently being used by any related components. Once the model itself is saved, this would naturally be the previous (earlier) revision, and no longer the latest.
Accessing the option to update related components that are referencing the symbol being re-saved.
If you want to keep all related components using the current revision of the symbol, disable this option. Only the model itself will then be saved.
Once you click OK in the Create Revision dialog, the modified symbol is saved back to the Workspace, and its associated temporary editor closed. All components referencing that symbol will be re-saved to use its new revision automatically (the next revision of each component is automatically created and the save performed).
Example of automatic update in action. Here, the graphics for a symbol have been changed. The component that references the symbol is automatically updated – re-saved into its next revision, to use the new revision of the symbol.
Downloading Saved Data
Download the data stored in a revision of a symbol by right-clicking on that revision (in the Explorer panel) and choosing the Operations » Download command from the context menu. The schematic library file will be downloaded into a sub-folder under the chosen directory, named using the Item Revision ID. The file can be found in the Released folder therein.
Access the Download command from the top-level entry for a symbol itself, to download the schematic library file stored in the latest revision of that symbol.
Click the Explore button in the Download from Server dialog, to quickly explore to the download folder.
Soft Deletion
When connected to a Workspace, flexible functionality is available for removing a symbol directly from within Altium Designer:
- From the Explorer panel – right-click on the symbol's entry in the panel and choose the Delete Item command from the context menu.
- From the Components panel – select the Symbols category (the Models option must be enabled in the panel's menu for accessing this category), right-click on the entry for a symbol and choose the Operations » Delete command from the context menu.
The Delete Items dialog will appear, in which to confirm the deletion. The action is actually a 'soft delete', whereby the symbol will be moved into the Trash area of the Workspace. The Trash is essentially a recycle bin into which any content within your Workspace can be moved (through a soft delete action). It is isolated from the rest of the Workspace.
With the soft-delete facility, you are able to delete a symbol that is currently being used.
Multiple symbols can be deleted in a single action. Select all required symbols using standard multi-select controls (Shift+Click, Ctrl+Click), then right-click and choose the deletion command from the context menu.
Soft deletion of a symbol from within the Explorer panel. The symbol will be moved to the Workspace's Trash area.
To proceed with the deletion, click the 
button. The symbol will be removed and a Deletion Summary dialog will confirm successful deletion. If there was an issue with deletion, this will be flagged to you.
The content deleted in this manner can be found on the Trash page of the Workspace's browser interface. Note that you can only view the content that you have personally soft deleted. Administrators will be able to see the full content of the Trash page – so all content that has been soft deleted.
Things to consider in relation to a soft deleted symbol:
- The symbol will not be available from your design software, or from within the Web interface.
- Anywhere the symbol was being used will reflect that the symbol has been deleted.
- A symbol can be restored, or permanently deleted from the Trash page, provided you have editing rights. Permanent deletion is only possible provided it is not being used by a parent Item.
Note that if you have soft deleted a symbol – moving it to the Trash – you can create a new symbol with that same name again. If you were to subsequently restore the original symbol, and the original name is taken, an integer suffix will be used, to keep its name unique within the Workspace.
Migrating Existing Model Libraries
Main page: Migrating Existing Libraries to Your Connected Workspace
Models can also be created in the Workspace as part of migration of existing libraries of components. Altium Designer, in conjunction with your connected Workspace, provides a streamlined, simple process to quickly migrate your existing libraries to that Workspace. The GUI to this process – the Library Migrator – presents an intuitive flow that takes initial selected libraries, and migrates them to your Workspace. Catering for all types of libraries relating to older component management methodologies – SchLib, PcbLib, IntLib, DbLib, SVNDbLib – the Library Migrator is the perfect solution to quickly building your company's Workspace component library so you can benefit from their many advantages – high-integrity, centralized storage and management, ease of design reuse, real-time supply-chain information.
The Library Migrator offers a minimalist Simple interface mode where the selected database and file-based component libraries are migrated to Workspace components through a single step, while the migrator automatically takes care of type classification, the target source folder, parameter inclusion and value type, and the transfer of all relevant data. The interface is also available in an Advanced mode that provides a full preview of the proposed library migration, and access to its related data and settings. And while the migration is a single-click process by default, the migrator also offers advanced configuration options through the Properties panel for enhanced control over exactly how that migration is performed.
Access the Library Migrator from any editor by choosing the File » Library Migrator command from the main menus.
While access to the Library Migrator is available in Altium NEXUS, should you wish to access a database or file-based library to make pre-migration tweaks, or access the Available Libraries list, you will need to enable the use of legacy component management methodologies. This functionality is disabled by default in Altium NEXUS, as it is not recommended. You can restore this functionality by enabling the
Legacy.UnManagedLibraries option in the
Advanced Settings dialog – accessed by clicking the
button, on the
System – General page of the
Preferences dialog. You will need to restart Altium NEXUS for the change to this setting to take effect.
All information that is present in an original source library is migrated to the Workspace components, including all referenced domain models (schematic symbols, PCB footprints, simulation models), parametric information, assigned part choices, datasheet files, etc. Component Templates are also created where necessary, and may then be refined and used for subsequent library migrations. If your original components have multiple PCB footprints defined, the Library Migrator will bring those models across and keep the current default footprint. And if you only work with PCB libraries – your only concern is PCB layout – then the Library Migrator supports migration of just those libraries, or it can be switched to a models only migration mode where specified models types are migrated from integrated or database libraries. Libraries that include multiple component types (monolithic libraries) are automatically detected and processed as well.
The Library Migrator in its Advanced mode – the full user interface to the component migration process.
While migration may seem daunting, the defaults have been defined to enable you to get your collection of Workspace components without having to change a thing – start the process and design with the fruits of the Migrator's labor. The system conducts and handles a number of validations, for example, to ensure no duplicate IDs for the resulting components, or to ensure no duplicate models or component templates are created, and that such entities are reused across (linked to) components where needed. And if issues do arise, the system flags them, with suggestions on how to resolve those issues, aiming to get the migration back on track as quickly, and as smoothly as possible.
