Components in a Workspace Connected to Altium Designer

Parent page: Workspace Content Types

Once all prerequisite domain models – such as schematic symbol, PCB footprint and simulation model – have been created and saved into your connected Workspace, a design component can be defined and saved into that Workspace for reuse in design projects. A company can authorize a set of such components (Component Items) – a Workspace library – that can be formally used by their designers. The Workspace becomes a single source of up-to-date and standardized component data for your entire design team. Parametric and faceted search capabilities allow you to find and place required parts efficiently and quickly. And you'll enjoy more capabilities provided by your Workspace, including the Where-Used feature, lifecycle and revision naming management, and component templates.

This document focuses on bringing the required pieces together to define and save a component into a Workspace.

Components are created directly from within the Workspace. Once a component has been created (and data saved into a revision of it), it can be reused in the creation of one or more designs.

Folder Type

When creating the folder in which to store components, you can specify the folder's type. This has no bearing on the content of the folder – saving a component will always result in a corresponding Component 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 components, set its Folder Type as Components, 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.

Content Type

When creating a target Component Item in which to store your component, ensure that its Content Type is set to Component, in the Create New Item dialog. If you are creating the Item in a Components type folder, this content type will be available from the right-click context menu when creating the Item.

Creating a component within a Components folder – while the correct Content Type is available on the context menu (Component command), using this will take you into item-less component creation mode. To create a traditional Item using the Create New Item dialog, choose the Other Item Type command from the menu instead.

To see your newly created component, which has yet to be defined and saved to the Workspace, either disable the Show only latest option (available from the menu accessed by clicking the button at the top of the Explorer panel), or switch the view for the folder from Components View to Classic View (available from the same menu).

Saving a Component Definition

Related page: Creating and Editing Content Directly through a Workspace

So far, we've discussed the support for a component in the Workspace, in terms of related folder and content types. Saving an actual defined component into a revision of a Component Item can be performed in a streamlined way.

A component can be edited and saved into the initial revision of a newly-created Component 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 Component Item, you have the option to edit and save the component 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 Component Editor will open, in its Single Component Editing mode, with the controls to define the component presented in the main design window. The document tab for the view will reflect the Name you have assigned to the component.

Example of editing the initial revision of a component, directly from the Workspace – the temporary Component Editor provides the controls with which to define your component (shown in its default Single Component Editing mode).

Use the Component Editor to define the component as required. The Editor supports two modes of operation – Single Component Editing mode (the default), and Batch Component Editing mode. For more information see Defining the Component.

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 Component Library Standard toolbar:

• – Save Active Document. Use this button to locally save any changes made to the component. 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 component to the Workspace, storing it within the initial (planned) revision of the target Component Item. The Edit Revision dialog will appear, in which you can change Name, Description, and add release notes as required. The editor will close after the save. The source component definition will be stored in the revision of the Item.

  A Save to Server control is also conveniently provided to the right of the component'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 editor will close, and nothing will be saved to the target Component 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 component's entry in the Projects panel.

The saved data stored in the Workspace consists of the source component definition. In the Explorer panel, switch to the Preview aspect view tab to see full definition data, including referenced models, component template (if used) and parametric information.

Browse the saved revision of the component, back in the Explorer panel. Switch to the Preview aspect view tab to see information including referenced models, component template (if used) and parametric information.

Item-less Component Creation

The use of Component Templates provides an efficient means for creating components using ratified templates, however there is a drawback. Since the Item is created first, the information in the template (i.e. naming scheme, revision scheme and lifecycle definition) are not assigned since the Component Item is already created. In order to alleviate this, the Workspace, in conjunction with Altium Designer, supports Item-less component creation. This does not mean an item is not created, but rather an instance of the Component Editor is accessed directly, which allows the template details to be applied prior to adding and saving the required component. The actual Component Item (and planned revision) is created as part of release preparation.

From the Explorer panel, Item-less component creation is available from within an existing folder for components (folder type must be Components). There are two ways to enter item-less component creation mode:

• By using the Create Item » Component command from the Item region's right-click menu.
• By clicking the button, located at the top-right of the panel.

Accessing Item-less component creation mode from within the Explorer panel. The current folder must be of type Components.

On entering this mode, a temporary (direct editing) instance of the Component Editor (in its default Single Component Editing mode) will be opened, ready to define the component. The default presentation and information loaded depends on whether a component template is involved.

• If the mode is accessed from a folder of components and that folder has a component template attached, then model and parametric data, as well as defined Lifecycle Definition, Revision Naming, and Component Naming, will be brought in from that template. The Default Folder will be the folder from which the mode was launched. If a default Name has been specified in the template, this will be used to name the component, and also appear in the tab for the Component Editor's document view. If no default name has been specified, the tab will display New Component, and the component's Name will be blank.
• If the mode is accessed from a folder of components and that folder has no component template attached, then a default component with default settings will be presented. If the source folder has a defined Item Naming Scheme, then this will be used to create the component's unique ID. The Default Folder will be the folder from which the mode was launched. All other definition information (models, parameters, component type) must be manually specified. The tab for the Component Editor's document view will display New Component, and the component's Name will be blank.

By way of example, we'll just consider the first scenario. After all, getting the component template used is why this mode was created. Just remember, that while the process will be very similar for the other scenario, you will just need to do more manual work if not using a template.

Example component created after launching the item-less component creation mode from a folder (Schottky) that has a component template assigned to it. The component is defined with the information from the template. Roll over the image to see the referenced Component Template.

Make any adjustments to the component as required, including the addition of Part Choices.

With the component defined, click the / button (on the Quick Access Bar) to save the component to the Workspace. The Edit Revision dialog will appear, in which you can change Name, Description, and add release notes as required. The editor will close after the save.

Your new component will be available to view in the Explorer panel, and also to browse for and work with, through the Components panel.

Defining the Component

Main pages: Single Component Editing, Batch Component Editing

A component is defined/edited using the Component Editor. This editor provides two different modes of operation:

• Single Component Editing mode – provides a streamlined interface when defining/editing a single component. This is the default mode when creating a new component, or editing a single revision of an existing component.

  
  Example showing definition of a component, with the Component Editor in its Single Component Editing mode.

  A new component can be quickly created, using the Component Editor in its Single Component Editing mode, by using the File » New » Component command, accessible from any editor, or by using the Operations » Create command, located on the right-click menu when browsing Workspace components through the Components panel.

• Batch Component Editing mode – provides the interface for defining/editing multiple components. You can access this mode by choosing the Tools » Switch to Batch Editor command, from the main menus of the Component Editor in its Single Component Editing mode. This mode is also accessed if you have selected multiple component revisions for editing, from the Explorer or Components panel. Each component definition will have a common set of parameters and links to required domain models. Batch editing comes into its own where it makes sense to manage components as a set, such as a set of chip resistors for example.

  You can use the Batch Component Editing mode to define/edit a single component, should you wish.

  
  Example showing definition of a component, with the Component Editor in its Batch Component Editing mode. While you can use this mode to edit a single component (as shown), its power really comes when editing multiple components that share the same parameters and models.

Referencing a Component Template

Related page: Component Template

Helping to streamline the creation of your components, Altium Designer, in conjunction with your Workspace, supports the use of Component Templates. Just as a schematic template can be used to predefine information on schematic sheets that reference it, a component template is referenced by a Workspace component, and provides predefined settings for use when defining that component.

Using a revision of a component template – or rather referencing one from the revision of a component you are currently editing – can be performed in the following ways.

When Creating a New Component

When creating a new component using the File » New » Component command from the main menus, you can choose the template in the Create new component dialog.

Quickly linking a component template from a listing of all available templates, when creating a new component.

Manually from within the Component Editor

Reusing a revision of a Component Template from the Component Editor, depends on the operating mode of the Editor.

In Single Component Editing Mode

When editing a single component in this mode of the Component Editor, choose the required Component Template from the drop-down menu associated with the Template field – part of the Advanced Settings grouping, in the Component region of the Editor. All component templates currently available in the same Workspace in which the component itself resides are listed – by name – with their latest revisions indicated in brackets. Choose the required template to have it applied.

Quickly linking a component template from a menu of all available templates, when editing the revision of a component using the Component Editor in its Single Component Editing mode.

In Batch Component Editing Mode

There are two ways of 'hooking up' a revision of a Component Template, to the component revision currently being edited:

• From the Template tab of the Document Options dialog (Edit » Document Options). Click the Choose button to the right of the Item Revision field. This gives access to the Choose Item dialog (an incarnation of the Explorer panel). Use this dialog to browse to, and select the revision of the required component template. After clicking OK, a link will be created between the revision of the component and the target revision of the component template. Evidence of this link can be seen back on the Template tab of the Document Options dialog.

  
  Manually linking a component to a revision of a component template, in the target Workspace.

  The component template being used can be changed at any time – click Choose and select a revision of a different component template.
  The status of the linked Component Template Item Revision is reflected on the Template tab of the Document Options dialog. If a newer revision of the linked Item is available, click the button, to use that latest revision.

• From the Add menu associated with the Required Models/Parameters region of the Component Editor. The Templates sub-menu lists all component templates – by name – currently available in the same Workspace in which the component itself resides, with their latest revisions indicated in brackets. Click on an entry to create a link to the latest revision of that component template. Once again, verification of the link can be seen on the Templates tab of the Document Options dialog.

  
  Quickly linking a component template from a menu of all available templates.

Inherited from the Components Workspace Folder

You can specify a Component Template to be automatically used for all components (and revisions thereof) stored within a Components folder within the Workspace.

Specify the required template using the Component Template field, when defining the folder's properties, in the Edit Folder dialog. The field's associated drop-down lists all component templates – by name - currently available in the same Workspace in which the Components folder itself resides, with their latest revisions indicated in brackets. Choose an entry to create a link to the latest revision of that component template, for each subsequent component created within that folder.

Specify a default component template, to be applied to all components created within the parent Components folder.

If a Component Template is chosen at the folder level, that same template will be used, by default, when components are created in child sub-folders below. This facilitates quick template inheritance to all components in child folders.

Impact on Component Models and Parameters when using a Component Template

When editing a revision of a component, and a revision of a Component Template is linked to/referenced, the following happens within the Component Editor, with respect to models and parameters:

• The models defined within the referenced template are added to the Models region (Single Component Editing mode) and Model Links region (Batch Component Editing mode).
• An existing referenced model will be kept, and the component will remain using that model, unless purposefully changed manually.

• The parameters defined within the referenced template are added to the Parameters region (Single Component Editing mode) and Required Models/Parameters region (Batch Component Editing mode).

  
  Example of parameters after linking to a revision of a component template, when using the Component Editor in Single Component Editing mode (left) and Batch Component Editing mode (right).

  All parameters originating from the referenced component template are distinguished by use of the icon (Single Component Editing mode) and icon (Batch Component Editing mode). In addition, and for Batch Component Editing mode only, the Show option for each template-based parameter follows the state of the corresponding Visible option in the template.
  Template-based parameters cannot be removed.
  You are free to add additional user-parameters as required.
• An existing user-defined parameter that has the same name as a parameter in the linked component template, will be replaced with the template version. Any existing value for that parameter will be kept (and not overwritten with the value in the template).

• In Batch Component Editing mode only, template-based parameters that are set to be shown are grouped together in the component definitions area of the editor, with Template Parameters used as the header text.

  
  Appearance of example template-based parameters in the area where the component definitions themselves are defined, when using the Component Editor in its Batch Component Editing mode.

• The value fields for template-based parameters that have been marked as read-only, will be non-editable. For all other template-based parameters, that have not been marked as read-only, you are free to change the values as required.

  With the Component Editor in Single Component Editing mode, a Read-only template parameter is distinguished in the Parameters region by use of the icon.

• If a template-based parameter has been marked as required, but has not been given a value in the template, its value field will appear with a red border (in Batch Component Editing mode) or containing the icon (in Single Component Editing mode), alerting you to the fact that a value is required for this parameter. You will not be able to save a component to the Workspace until values are defined for all required parameters.

  With the Component Editor in Single Component Editing mode, a required template parameter is distinguished in the Parameters region by use of the icon.

Parameter List Templates

If you are not using Component Templates, you can still create predefined listings of parameters through the Component Editor's support for customizable Parameter List Templates. These simple, humanly-readable files can be built with a list of required parameters, that can then be loaded into the editor with a single click.

Parameter list templates can be found in the Templates sub-menu – accessed by clicking the Add control at the bottom of the Required Models/Parameters region. A number of predefined templates are available, covering parameter sets associated with capacitors (Capacitor), resistors (Resistor), diodes (Diode) and transistors (Transistor).

Access parameter templates from the menu associated to the region's Add control.

Click on the template you wish to use – the parameters defined within that template will be added to the region.

Adding a set of parameters for use by your component(s) is expedited through the use of parameter templates.

Template Definition

A parameter template is defined in a Component Library Template file (*.cmplib_template). To be recognized by the system, and therefore appear in the Templates sub-menu within the Component Editor, these files must reside in the Templates folder of your Altium Designer installation (\Users\Public\Documents\Altium\AD<VersionNumber>\Templates for a default installation).

The template definition is straightforward, consisting of the name for the template (as it is to appear in the sub-menu) enclosed in square brackets, followed by a listing of the required parameters, in the format <ParameterName>=. By way of example, the predefined template for resistors – resistor.cmplib_template – has the following definition:

[Resistor]
Category=
Manufacturer=
Manufacturer Part Number=1
Mounting Type=
Temperature=
Package Type=
Package Reference=
RoHS=
Temperature Coefficient=
Tolerance=
Weight=
Height=
Value=
Power=
Resistance=
Composition=

Re-Saving a Component

At any stage, you can come back to any revision of a component in the Workspace, and edit it directly:

• From the Components panel – right-click on the entry for a component and choose the Edit command from the context menu.
• From the Explorer panel – right-click on the revision and choose the Edit command from the context menu.

Once again, the temporary Component Editor will open – in its Single Component Editing mode – with the component definition contained in the revision opened for editing. Make changes as required, then save the component into the next revision of the Item.

Accessing the command to launch direct editing of an existing component revision – either from the Components panel, or the Explorer panel.

Downloading Component Source

You also have the ability to download one or more components from your Workspace, into a Zip archive file containing source symbol and model libraries, and a source Integrated Library Package (*.LibPkg). This could be used to quickly generate an integrated library containing your chosen component(s). And when placing components from such an Integrated Library, the actual links are back to the components in the Workspace. This gives you the ability to effectively use your company's components in an offline fashion, while ensuring the design still maintains a true connection to those components in the source Workspace.

To be able to use this functionality in Altium NEXUS, 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.

From the Components panel, the process to download into a Zip file is as follows:

1. Browse to/filter your components using the panel's various features (Categories, faceted parametric filtering, etc).
2. Select the component(s) you want to include in the download. You can include as many different components in the download as required.
3. Right-click on an entry in the selection and choose the Operations » Download command from the context menu.
4. In the Save As dialog, specify the name, and location, for the generated Zip file. By default, the file will be named in the format Components - <Date> - <Time>.zip.
5. Once ready, click the Save button to proceed with the download, and generation of the Zip file. An Integrated Library Package (*.LibPkg) will be created, with source SchLib (with symbols, parameters and model links) and PcbLib (with footprint models) files generated and added. This is then compressed into the Zip file, which is generated in the specified folder. An information dialog will confirm successful generation of the file.

From the Explorer panel, the process to download into a Zip file is as follows:

1. Browse to the folder containing the component(s) you want to download.
2. Select the revision of the component(s) you want to include in the download. You can only choose one revision of a particular component (typically the latest revision), but can include as many different component in the download as required.
3. Right-click on an entry in the selection and choose the Operations » Download command from the context menu (if downloading multiple components, the command will appear as Operations » Download selected component to zip).
4. In the Save As dialog, specify the name, and location, for the generated Zip file. By default, the file will be named in the format Components - <Date> - <Time>.zip.
5. Once ready, click the Save button to proceed with the download, and generation of the Zip file. An Integrated Library Package (*.LibPkg) will be created, with source SchLib (with symbols, parameters and model links) and PcbLib (with footprint models) files generated and added. This is then compressed into the Zip file, which is generated in the specified folder. An information dialog will confirm successful generation of the file.

Example download (albeit a single component!) into a Zip file, in this case from the Components panel.

Soft Deletion

When connected to a Workspace, flexible functionality is available for removing a component directly from within Altium Designer:

• From the Components panel – right-click on the entry for a component and choose the Operations » Delete command from the context menu.
• From the Explorer panel – right-click on the component's entry in the panel and choose the Delete Item 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 component 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.

Soft deletion of a component, along with its associated symbol and footprint, from within the Explorer panel. The content will be moved to the Workspace's Trash area.

To proceed with the deletion, click the button. The content 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 component:

• The component will not be available from your design software, or from within the Web interface.

• Anywhere the component was being used will reflect that the component has been deleted.

  
  Example of a soft deleted component being flagged as such elsewhere in the software.

• A component 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 (on a managed schematic sheet, or within a design).

Migrating Existing Component Libraries

Main page: Migrating Existing Libraries to Your Connected Workspace

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.

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.