Managed Schematic Sheets in an Altium Vault_AD

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 reusable 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 Designer, in conjunction with Altium Vault, caters for the ability to create Managed Schematic Sheet Items in an Altium Vault. Such Items are created directly from within the target vault. Once a Managed Schematic Sheet Item has been created (and data released into a revision of it), and its lifecycle state set to a level that the organization views as ready for use at the design level, it can be reused in future board-level design projects.

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 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.

Folder Type

When creating the folder in which to store Managed Schematic Sheet Items, you can specify the folder's type. This has no bearing on the content of the folder - releasing a schematic sheet will always result in a corresponding Managed Schematic Sheet Item. 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 Managed Schematic Sheet Items, set its Folder Type as Managed Schematic Sheets, 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 vault!

Item Type

When creating a target Managed Schematic Sheet Item in which to store your schematic sheet, ensure that its Content Type is set to Managed Schematic Sheet, in the Item Properties dialog. If you are creating the Item in a Managed Schematic Sheets type folder, this Item type will be available from the right-click context menu when creating the Item.

Creating a Managed Schematic Sheet Item within a Managed Schematic Sheets folder - the correct Content Type is available on the context menu.

Releasing a Schematic Sheet

So far, we've discussed the support for a Managed Schematic Sheet Item in the vault, in terms of related folder and item types. Releasing an actual defined schematic sheet into a revision of such an item can be performed in a single streamlined way.

A schematic sheet can be edited and released into the initial revision of a newly-created Managed Schematic Sheet Item, courtesy of the vault's support for direct editing. Direct editing frees you from 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 released (or 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.

When you create a Managed Schematic Sheet Item, you have the option to edit and release a schematic sheet into the initial revision of that item, after creation. To do so, simply enable the option Open for editing after creation, at the bottom of the Create Item dialog (which is enabled by default). The Item will be created and the temporary Schematic Editor will open, presenting a .SchDoc 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>.SchDoc (e.g. SCH-001-0001-1.SchDoc).

Example of editing the initial revision of a Managed Schematic Sheet Item, directly from the vault - the temporary Schematic Editor provides the document with which to define
your schematic sheet.

Use the document to define the schematic sheet as required. 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). For more information see Working with Vault Components.

The Schematic Standard toolbar provides three relevant controls when direct editing:

•  - Save Active Document. Use this button to save the changes made to the document. This is required before you can release the document back to the vault.
•  - Release Document. Use this button to release the defined schematic sheet to the vault, storing it within the initial (planned) revision of the target Managed Schematic Sheet Item. The Create Revision dialog will appear, in which you can change Comment, Description, and add release notes as required. The document and editor will close after the release. The document containing the source schematic sheet, *.SchDoc, will be stored in the revision of the Item.
•  - Cancel Editing. Use this button if you wish to cancel editing. The document and editor will close, and nothing will be released to the target Managed Schematic Sheet Item.

The released data stored in the vault consists of the source schematic sheet, defined in the Schematic Document file (<Item><Revision>.SchDoc), as well as any associated harness definition files (*.Harness). In the Vaults panel, switch to the Preview aspect view to see a graphical representation of the sheet, along with a listing of its constituent components.

Browse the released revision of the Managed Schematic Sheet Item, back in the Vaults panel. Switch to the Preview aspect view to see a graphical representation, and a
listing of the child Component Item Revisions.

The child components used on the sheet can also be browsed from the Children aspect view. Double-click an entry to cross-probe, right-click to access a set of component-related commands.

Browse the constituent components on the managed sheet, through the Children aspect view.

Reusing a Managed Schematic Sheet Item

Related pages: The Managed Project and Releasing the Design, Controlling Access to Vault Content

Once a schematic sheet has been released to an Altium Vault, and its lifecycle state set to a level that the organization views as ready for use at the design level, that sheet can be reused in future board-level design projects. And keeping to the use of the vault as the source of all content in and for a design, it is good practice to reuse your managed sheet content in Managed Projects - which themselves are under the vault's wing.

It is the way you include a Managed Sheet in the current design that lets Altium Designer know it is not a regular schematic sheet. You add a regular schematic to your project via the File menu, whereas you add a Managed Sheet to your project by placing it from the vault, just like you were placing a vault component. Placement is performed from Altium Designer's Vaults panel.

Prior to Placement...

Placing a vault-based Managed Sheet truly is simplicity itself. But before you do anything, there are a couple of points to note:

• A Managed Sheet's sheet symbol cannot be placed onto a free schematic, the target sheet must be part of a project.
• Ensure that the schematic sheet that is to receive the associated sheet symbol is open in Altium Designer and is the active document. If documents are open across multiple windows, ensure also that the window containing that active schematic document has focus.

Placement

To place from the Vaults panel:

1. Browse or search for the Managed Schematic Sheet Item you wish to place.
2. Right-click on the specific revision of the Managed Schematic Sheet required (typically the latest, in which case just right-click directly on the top-level Item entry).
3. Choose the Place command.

A sheet symbol that references the sheet will float attached to the cursor - just pick a ball-park spot on the active schematic sheet and click to effect placement. You can fine tune and nudge it into its final location at a later stage.

As you place the sheet symbol, Altium Designer copies the Managed Sheet that the sheet symbol represents, from the vault into the project folder, within a sub-folder called \Managed\Sheets. A copy of each Managed Sheet is stored here, each within its own sub-folder identified by a system-generated unique identifier (GUID).

Placement of a Managed Sheet is similar to placement of a component. Right-click on the desired Item Revision and choose the Place command - a sheet symbol representing
the Managed Sheet is available on the cursor for placement into the design.

Drag and Drop from the Vaults Panel

For more express placement of your Managed Sheets from the Vaults panel, Altium Designer provides the ability to drag & drop revisions of Managed Schematic Sheet Items directly onto the active schematic document.

Simply browse a connected vault for the required Managed Schematic Sheet Item to be placed. Placement involves a specific revision of that Item, so be sure to expand the main Item entry to list all of its available revisions. Then simply click on the required revision and drag an instance of it onto the schematic sheet.

Drag the required revision of a Managed Schematic Sheet Item from the Vaults panel...and drop it onto the active schematic document.

Re-Releasing a Managed Schematic Sheet Item

At any stage, you can come back to any revision of a Managed Schematic Sheet Item in the vault, and edit it directly. Simply right-click on the revision and choose the Edit command from the context menu. Once again, the temporary editor will open, with the schematic sheet contained in the revision opened for editing. Make changes as required, then commit the release of the document into the next revision of the item.

Accessing the command to launch direct editing of an existing revision of a Managed Schematic Sheet Item.

Downloading Released Data

Download the data stored in a revision of a Managed Schematic Sheet Item by right-clicking on that revision and choosing the Operations » Download command from the context menu. The applicable file(s) will be downloaded into a sub-folder under the chosen directory, named using the Item Revision name. The file can be found in the Released folder therein.

Batch Releasing File-based Schematic Sheets

If you have a set of file-based schematic schematic sheets (*.SchDoc) that you need to release to a target Altium Vault quickly, and simultaneously, then you can use Altium Designer's Release Manager. Use it to batch-release schematic documents in a nominated source folder location.

Accessed the Release Manager dialog by running the File » Release Manager command.

Release schematic sheets, stored in one or more source documents, using the Release Manager.

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. Files 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 (default is SCH-{00000}) 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.