Releasing a Schematic Sheet to a Vault

Parent article: Design Content Management

Being able to re-use design content is something that all product development companies want, and can greatly benefit from. Not only does reuse save time, being able to easily re-use a section of a previous design means that all the qualification and testing of that part of the design is done. Design reuse is much more than copy and paste though, true reuse requires the content to be locked down so you're guaranteed that it is the same as before. No quick edits to change the color of a component or a tweak to a resistor value, working with reuse content must be like working with off-the-shelf components; place the content, wire it in, and it works just like it did last time.

Altium's Design Data Management System caters for the ability to formally release a schematic sheet (or tree of sheets), along with any associated Harness Definition files, into a target Schematic Sheet Item (and revision thereof) in an Altium Vault. Once the sheet has been released, and its lifecycle state set to a level that the organization views as ready for use at the design level, the sheet – which is now referred to as a Managed Sheet – can be reused in future board-level design projects.

Like vault components, Managed Sheets are placed from the vault into the current design. Like vault components, they can be revised if needed, with full control over the revision process. And like vault components, their lifecycle can also be managed (ready for prototype, for production, and so on), reflecting their real 'usability' state.

Just What is a Managed Sheet?

A Managed Sheet is a standard Altium Designer schematic sheet containing components and wiring, that has been stored in an Altium Vault, so it can be re-used in other designs. It is created and edited like any other schematic sheet. The Managed Sheet concept is not limited to a single schematic sheet either, you can place a Managed Sheet in your design that is the top of a tree of other Managed Sheets.

The decision to move from Device Sheets to Managed Sheets comes when there is a desire to make the transition from re-useable content to managed re-useable content – that is, when there is a desire or need to be able to control the release, revision status and lifecycle state of that design content.

By making it managed content you can be sure that the revision of a Managed Sheet that you use in a design can be easily identified and traced back to its source whenever needed. And because it is managed content it can be revised and updated when needed; and the usage relationships can all be traced, both down to the components on that sheet, and up to the designs that use that sheet. This ensures you have all the information needed to decide if that revised sheet must be pushed through to existing designs, or if a particular design must continue to use the previous revision.

Creating a Managed Sheet

Related article: Vault-Based Components

A defined schematic sheet on the design side is mapped to a Schematic Sheet Item in an Altium Vault. Each release of the sheet stores the data into a new revision of that Item.

Simply use Altium Designer's Schematic Editor to create the sheet of reusable design circuitry as required, using vault-based components to take full advantage of the managed content system that the vault provides.

Example schematic sheet of reusable design circuitry, defined ready for release to an Altium Vault.

You can now proceed to release the sheet. To do so requires the following steps:

1. Link the sheet to the required revision of a target Item in a target Altium Vault. The Item must be of type altium-schematic-sheet, and the revision in which to release the sheet data must be in the Planned state.
2. Release the sheet into that targeted Item-Revision.

Replacing Unmanaged Components with Managed Components

Related article: Managing Vault Items with the Item Manager

Because Managed Sheets are stored in an Altium Vault, the components on them should also be stored in the vault. That way, you get the full benefit of the managed content system that the vault provides, including being able to identify and locate all the components used on the Managed Sheet (the Children), and also being able to identify and locate which designs the Managed Sheet has been used in (Where-used).

If the sheet of reusable design circuitry is an existing schematic sheet, or device sheet, it is highly likely that the components on it are currently unmanaged. In other words, they are not sourced from an Altium Vault. So before releasing the sheet to the target vault, these components need to be replaced by their managed equivalents - vault components that have already been released to the vault.

Altium Designer's Item Manager (Tools » Item Manager) can detect all unmanaged components in the sheet (or project). In the Item Manager dialog, enable the Unmanaged Items and Components options, from the Show menu, to display which of the components have not come from a vault. The Lifecycle column will list all components that are not currently vault components, using the state [Not Managed].

Use the Item Manager to detect unmanaged components on the source schematic sheet.

Replacement can either be performed by manually choosing vault Items to use, or in a more automated fashion, using the manager's auto-matching feature. The latter works by taking the unmanaged design components and attempting to match each one with a managed Component Item in a connected vault. The matching process takes the Design Item ID of an unmanaged design component and compares it against the Comment property of managed Component Items in a vault. When a match is found, that managed Component Item will be proposed for the update.

To run this process:

1. Confirm that the Update option is enabled for those components that need updating.
2. Click the Auto-Match Unmanaged button.
3. The Link Unmanaged Components To Vault dialog will appear, with the results of the matching process, grouped by Item-Type. The Messages column will detail if a match has been found or not. If the Message for a component warns that there are multiple matches found, select that component, then click the Choose Alternative Component From Vault button. Use the subsequent dialog to select the required component Item-Revision.
4. Click OK to accept the links – the information in the New Settings region of the Link Unmanaged Components To Vault dialog will be copied to the New Settings region back in the Item Manager.

Proposed changes are ready to be implemented.

Once changes have been set up as required, those changes need to be implemented. This is done through an Engineering Change Order (ECO). The drop-down menu associated with the ECO button, at the bottom of the Item Manager, provides commands for generating/applying the required change order. Executing the ECO will replace each unmanaged component with the chosen managed component. The Sheet is now ready to be saved and released to the vault.

Linking the Sheet to a Vault

Before any data can be added to a vault, there must be an Item defined in the vault to 'hold' that data. The Item is created before releasing the schematic sheet into the vault. The link to the target vault and Item Revision therein, is stored as part of the schematic.

The first step is to link the sheet to the vault, using the File » Link Sheet to Vault command. The linkage is stored as part of the Document Options for the sheet, which is why the Document Options dialog will open, with the Link To Vault option enabled.

Controls for linking the source schematic sheet to a Schematic Sheet Item in a target vault.

Clicking the Choose button to the right of the Item Revision field will give access to the Choose Item dialog – essentially a trimmed incarnation of the Vaults panel. The field at the top-left of the dialog indicates which vault you are currently exploring. To select a different vault, click the  icon to the left of the vault name (or on the vault name itself) to access a menu of top-level vault management controls. This menu displays all vaults that you currently have an active connection to.

With the required target vault active, you can either drill down through its folder hierarchy to select the required existing Item, or create the folder and/or Item as required, on-the-fly. Ensure that the Item-Revision chosen – which will receive the released data – is in the Planned state.

Manually linking the source schematic sheet to a planned revision of a Schematic Sheet Item, in the target vault.

Folder Type

Whether you have created a Schematic Sheet Item in the target vault beforehand, or are creating it in situ at the time of sheet linking, you will need to first create the folder in which that Item will reside. As part of folder creation, the folder's type can be specified. This has no bearing on the content of the folder – releasing schematic sheets will always result in Schematic Sheet Items. It simply provides a visual 'clue' as to what is stored in a folder and can be beneficial when browsing a vault for particular content. To nominate a folder's use as a container for Schematic Sheet Items, set its Folder Type as altium-managed-sheet-catalog.

Specifying the folder type - its intended use - provides visual indication of the content contained within that folder while browsing the vault.

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 or the content type. Using a default naming scheme, the software will automatically assign the next available unique ID, based on that scheme, having scanned the entire vault and identifiers of existing Items. This can be a great time-saver when manually creating Schematic Sheet Items prior to release.

A custom scheme can also be defined for a folder, simply by typing it within the field, ensuring that the variable portion is enclosed in curly braces (e.g. SHEET-001-{C000}).

The Item Naming Scheme of the parent folder is applied to the Unique ID for each Item
created within that folder.

Item Lifecycle Definition and Revision Naming

When defining the Schematic Sheet Item, to which the source schematic sheet is linked, be sure to specify the type of lifecycle management to be used for the Item, and the naming scheme employed for its revisions, respectively.

Specify the required schemes in the Item Properties dialog, using the Lifecycle Definition and Revision Naming Scheme fields respectively.

Selecting the Lifecycle Definition and Revision Naming schemes for a manually created Item.

Verifying the Link is Established

Once the required revision of the Schematic Sheet Item in the target vault is chosen, clicking OK in the Choose Item dialog will create the link between source sheet and target Item. Evidence of the link can be seen back in the Document Options dialog. Close the dialogs and save the source document – so that the link information is saved to the sheet.

Evidence that the source schematic sheet is now linked to an Item in the vault.

Performing the Release

With the link to the target vault and Item-Revision in place, the process of releasing the source schematic sheet into the vault can proceed. Select the File » Release To <TargetVaultName> command. When the data has been prepared to be added to the vault, the Release confirmation dialog will appear. This dialog also includes a field to add any pertinent release notes. Click Yes to commit the sheet to the vault.

After its release, the Revision State is updated in the Document Options dialog, which will now show Released (when using basic lifecycle management), or New From Design (when using another default management scheme). Be sure to save the document. Click the Show in Explorer button to browse the released sheet directly in the vault using the Vaults panel.

Browsing the released Schematic Sheet Item (Managed Sheet) in the vault, using the Vaults panel.

The released data stored in the vault consists of the .SchDoc file.

With the sheet released, it can now be reused in new design projects.

Re-releasing the Source Schematic Sheet

With the source schematic document linked to the vault and Schematic Sheet Item therein, re-releasing the sheet – to take into account any modifications – is a straightforward process:

1. Make the changes to the source schematic document as required.
2. Create a new Planned revision for the linked Schematic Sheet Item. This can be done from the Lifecycle view for the Item, in the Vaults panel, or from the detailed view for the Item. With the schematic document active in the workspace, the latter can be accessed from the Document Options dialog by clicking the Details button (to the far right of the Item Revision field).
3. Choose this new Item Revision in the Document Options dialog.
4. Save the SchDoc file.
5. Use the File » Release To <TargetVaultName> command.

Streamlined Re-release through File-less Editing

Main article: File-less Editing in an Altium Vault

File-less editing frees you of the shackles of separate version-controlled source data. You can simply edit a supported Item type using a temporary editor loaded with the latest source direct from the vault itself. And once editing is complete, the entity is re-released 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 Altium Vault handles it all, with the same great integrity you've come to expect, and in a manner that greatly expedites changes to your data.

Releasing Multiple Schematic Sheets

Related article: Batch Releasing to a Vault with the Release Manager

Releasing single schematic sheets to a target vault can be a tedious task – especially since release of a single schematic requires that file (SchDoc) to be open and active in Altium Designer. This is also the case if changes have been made affecting an array of source schematic documents, that need to be re-released into a new revision of each target Schematic Sheet Item.

To facilitate the release of multiple schematic sheets to a target vault simultaneously, Altium Designer provides a Release Manager (File » Release Manager). Use it to batch-release schematic documents in a nominated source folder location.

Setting up for release couldn't be simpler:

• Set the Document Type to SCHDOC.
• Point to a top-level folder containing the schematic documents you want to release. Documents can be stored in sub-folders within this folder.
• Choose the target vault.
• Choose to create a top-level folder in the vault based on the nominated top-level Windows folder, or choose an existing vault folder. You can optionally create sub-folders in the nominated vault folder, for each Windows sub-folder. Additionally, you can opt to create a vault folder for each source schematic document.
• Use the Default Options for New Released Schematic Documents region of the Release Manager to control how required new Items are created as part of the release process – in terms of Lifecycle Definition, Item Naming and Item Revision Naming schemes, and starting index.
• Hit the Analyze Folders button.

Analysis of source folders and target vault folders (and Items) based on your chosen options will be performed and the source schematic documents detected will be listed. For each entry, the target Item will be displayed, its current and/or next revision (as applicable) and the action that will be performed by the release process.

Enable the schematic documents that you want to release and then click the Prepare Items and Documents button to effectively commit the link information to the source schematic documents involved in the release. Once saved, proceed with the release by clicking the Release Items button.

Batch-release schematic documents using the Release Manager.