Altium Designer Documentation

Managed Schematic Sheets in an Altium Vault

Modified by Jason Howie on Apr 11, 2017

Parent page: Design Reuse

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.

Managed Sheets differ from Device Sheets in that they are stored in an Altium Vault, where Device Sheets are stored in a folder on a hard drive. As such, they enjoy the benefits attributed to managed vault content, including revision and lifecycle management, and of course secured integrity.

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!

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 (SSC - Schematic Sheet Collection) or the content type (SCH - Schematic Document):

  • $CONTENT_TYPE_CODE-001-{0000} - for example, SCH-001-0001.
  • $CONTENT_TYPE_CODE-001-{A00} - for example, SCH-001-A01.
  • $FOLDER_TYPE_CODE-001-{0000} - for example, SSC-001-0001.
  • $FOLDER_TYPE_CODE-001-{A000} - for example, SSC-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 vault and identifiers of existing Items. This can be a great time-saver when manually creating Managed 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-{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 Items within that folder.

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.

When defining a Managed Schematic Sheet Item, be sure to specify the type of lifecycle management to be used for the Item, and the naming scheme employed for its revisions, respectively.

Control over which Item 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. For a newly-installed vault, the default schemes assigned for use by a Managed Schematic Sheet Item are: Simple Lifecycle and 1-Level Revision Scheme, respectively.

Once a template definition has been released into the initial revision of a Managed Schematic Sheet Item, these schemes cannot be changed for that particular Item.

Specify the required schemes in the Item Properties 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 Managed Schematic Sheet Item 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 Item.

Observing standard revision naming schemes and lifecycle definitions, across the various types of design item in a vault ensures smooth, consistent management of those items.
It is a good idea to add a comment and description as part of the Item's definition. This information is used when searching the vault and enables quick identification of what a Managed Schematic Sheet Item offers.

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 ability to use vault-based components to build larger design building blocks enables the design-flow to become ever-more streamlined, and at a higher level of abstraction. The designer, just like picking parts off a shelf, simply reuses these managed sheets of design functionality as constituent components of the bigger design project. And the more managed sheets of such circuitry that have been created and released into the vault, the more functionality the designer has access to, which in turn boosts productivity for subsequent designs.

When it comes to the design of a managed sheet, the application of tuned standards not only aid in readability of the sheet, but bring a strong level of design consistency and uniformity. So not only a consistency presentation-wise, but also adherence to certain best-practice design principles. The following sections take a closer look at a suggested naming convention for managed sheets, as well as some of the key standards that might be followed in their design.

Naming Convention

In terms of naming, one suggestion is that each managed sheet is named according to the primary, or key component that it features. This name is the part's order code (the code used when ordering it from a vendor). Example managed sheet file names might be:

  • MAX3062EEKA.SchDoc - featuring a MAX3062EEKA 20Mbps RS-485 Transceiver, from Maxim.
  • BMP085.SchDoc - featuring a BMP085 Digital Barometric Pressure Sensor, from Bosch.
  • RTL8201CL.SchDoc - featuring an RTL8201CL Single-Port 10/100M Fast Ethernet PHYceiver, from Realtek.

The sheet title can be used to concisely describe the functionality of the circuit captured by the sheet. Typically, the key component name will also be included in this title.

Example managed sheet, featuring a BMP085 component.

Design Standards

When it comes to populating a blank schematic sheet, designers are rather chef-like in nature, each has their own signature way of doing things. Presentation-wise, for example, different designers will adopt different styles, layout preferences, use of color, and so on. After all, if all designers across the planet presented schematic circuitry in the exact same fashion, the design world would take on a mundane, monochromatic-like appearance! The key is to adopt a method of capture and presentation that is consistent across your own design teams.

Now, in saying that, there are some key design principals that, when adopted, really do aid not only the consistency of the managed sheets produced, but are fundamental to the concept of design for reuse itself. The following are some suggested principles:

  • Each managed sheet features a single or small group of key components focusing on a specific function.
  • All possible supporting circuitry will be included in the sheet.
  • Parts of the design that can be configured in multiple ways can be refactored to parent or sub-sheet within reason, allowing the sub-sheet behavior to be configured from the parent without adding unnecessary structural overhead.
  • Multi-purpose signals are passed to parent sheets using reasonable and generic signal naming, allowing them to be re-mapped to their specific purpose.
  • Ensure readability of the single standalone managed sheet is preserved, while allowing a designer to easily understand how it would be implemented as an element in their design.
  • Use of consistent naming, presentation and design standards.

In terms of designing for reuse, the following suggested items are particularly relevant and important to capture at the managed sheet level:

  • The use of signal harnesses where possible, since the standard harness is itself a reusable design element.
  • No labeling of local nets – so avoiding the use of Net Labels – since doing so actually makes it harder to manage connectivity through the design in which the managed sheet is used. The most common exception to this however, is the requirement of such labeling when creating buses.
  • All power ports connected to a port sheet interface and passed to the parent sheet – local power ports are avoided to prevent confusion.
  • Port direction and I/O type is strictly set according to the signal direction with the exception of Power nets (these will be unspecified). Where signal direction is not specified, Bidirectional is used.
  • Using a standard set of signal names, using generic names where possible (e.g. 5V0 instead of 5.0V/5V/5Volts). There is a certain degree of flexibility here as well, since connections are explicit through the use of strict hierarchy across all design projects. This allows names to be defined differently for any two connected objects, at different levels of the design hierarchy, because their connection is explicit.
  • Using a standard set of sheet-level parameters.

Another suggested addition to a managed sheet is that of a section to highlight the key component on the sheet, in terms of its manufacturer, and an at-a-glance listing of its key features. This can prove invaluable to a designer when assessing its merit for inclusion into a new design.

Features of the key component listed alongside the design circuitry.

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.

Click on the hyperlink entry for a child Component Item Revision to cross-probe to it in the Vaults panel. The Child Items area also provides a right-click context menu with commands for working with a child Component Item Revision.

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.

Using controlled access to vault content, in conjunction with suitable lifecycle schema, authorized personnel (librarians, senior design management) can ratify, and make available, only those Managed Sheets that are to be used in designs. This allows the designer to design-away, reassured that they are using only those sheets of reusable design circuitry authorized to be used.

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.
When working with Altium Designer across multiple windows, if the Vaults panel is docked in any mode to a window without the target schematic in it, the Place command will remain grayed-out. This is because clicking within a docked panel focuses the window to which that panel is attached. With the panel floating however, the required Altium window can be focused (the one with the active target schematic), and that window will keep focus when working inside the panel.

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).

The GUID-named sub-folder in which the instance of the Managed Sheet is downloaded and stored must not be edited/renamed in any way.

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.

Once a Managed Sheet has been placed into a design, re-compile the project for it to appear in the project structure and to be able to drill down into that sheet.

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 and drop the top-level entry for a Managed Schematic Sheet Item itself, to place an instance of the latest revision of that Item.

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.

Right-clicking on the top-level entry for an Item itself, will edit the latest revision of that 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.

Access the Download command from the top-level entry for a Managed Schematic Sheet Item itself, to download the applicable file(s) stored in the latest revision of that Item.
Click the Explore button in the Download from Vault dialog, to quickly explore to the download folder.

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.

The Release Manager is considered to be a legacy tool.

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.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.


Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Sounds exciting! Did you know we offer special discounted student licenses? For more information, click here.

In the meantime, feel free to request a free trial by filling out the form below.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.