Altium Designer Documentation

Managed Schematic Symbols in an Altium Vault

Modified by Jason Howie on Apr 11, 2017

Parent page: Vault-based Domain Models

From a designer's perspective, a vault component (Component Item) 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 vault component doesn't contain the domain models themselves, but rather links to these models. These links are specified as part of the source component definition - from which the released Component Item is generated. As such, before you can delve into the process of defining and releasing vault components, you must first ensure that all the domain models themselves have been created and released.

Altium Designer, in conjunction with Altium Vault, caters for the ability to create and manage Symbol Items in an Altium Vault. Such Items are created directly within the target vault. Once a Symbol 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 the creation of one or more vault components.

Folder Type

When creating the folder in which to store Symbol Items, you can specify the folder's type. This has no bearing on the content of the folder - releasing 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 vault for particular content. To nominate a folder's use as a container for Symbol Items, 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 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 (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 vault and identifiers of existing Items. This can be a great time-saver when manually creating Symbol 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. 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 Items within that folder.

Item 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 Item Properties dialog. If you are creating the Item in a Symbols type folder, this Item type will be available from the right-click context menu when creating the Item.


Creating a Symbol Item within a Symbols folder - the correct Content Type is available on the context menu.

When defining a Symbol 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 Symbol Item are: Component Lifecycle and 1-Level Revision Scheme, respectively.

Once a schematic symbol has been released into the initial revision of a Symbol 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 Symbol 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 Symbol Item offers.

Releasing a Schematic Symbol

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

A schematic symbol can be edited and released into the initial revision of a newly-created Symbol 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 Symbol Item, you have the option to edit and release a schematic symbol 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 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-001-0003-1.SchLib).


Example of editing the initial revision of a Symbol Item, directly from the vault - 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 the Schematic Symbol.

One important thing to observe is that only the symbol graphics need be defined - the representation of the higher-level vault-based component within the schematic editing domain. It is not a 'schematic component' as defined for use in integrated libraries, where other models and parameters are defined as part of that schematic component. A vault-based 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.

The Sch Lib 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 symbol to the vault, storing it within the initial (planned) revision of the target Symbol 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 library document containing the source schematic symbol, *.SchLib, 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 Symbol Item.

The released data stored in the vault consists of the source schematic symbol, saved in a Schematic Library file named using the Symbol Item's Comment. In the Vaults panel, switch to the Preview aspect view to see the symbol graphics.


Browse the released revision of the Symbol Item, back in the Vaults panel. Switch to the Preview aspect view to see the symbol graphics.

Reusing a Managed Symbol Item

Related page: Managed Components in an Altium Vault , Controlling Access to Vault Content

Once a schematic symbol 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 symbol can be reused in the creation of one or more vault components . When directly editing a Component Item from a vault, a Symbol Item revision is added for use to the resulting Component Library'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 in the Component Library document. Assignment is simply a case of specifying which links are required for each definition.


Example of referencing a revision of a Symbol Item as a model link in a Component Library, when direct editing the definition for a Component Item (vault component).

You can edit a Symbol Item revision directly from the Model Links region by right-clicking and choosing the Edit command from the context menu.

Re-Releasing a Symbol Item

At any stage, you can come back to any revision of a Symbol 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 library (containing the source schematic symbol) 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 Symbol Item.

Updating Related Component Items

When you make a change to a vault-based domain model - be it a symbol, footprint model, or simulation model - the moment you release that change into a new revision of the model's Item, any Component Items 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-release those components, with the respective model links updated to use the latest revisions available. To streamline this process, Altium Vault, in conjunction with Altium Designer, facilitates the ability to update related Component Items - at the point of re-releasing a model Item - after having made any modifications to that model through the direct editing feature.

The option to perform this update to the parent Component Items, can be found in the Create Revision dialog, that appears when releasing the modified symbol back to the target Altium Vault. This option - Update items related to <ModelItemRevision> - is enabled by default.

<ModelItemRevision> is the current revision of the model Item, that is, the revision currently being used by any related Component Items. Once the model itself is released, this would naturally be the previous (earlier) revision, and no longer the latest.


Accessing the option to update related Component Items, that are referencing the Symbol Item
being re-released.

If you want to keep all related Component Items using the current revision of the Symbol Item, simply disable this option. Only the model itself will then be released.

Once you click OK in the Create Revision dialog, the modified symbol is released back to the vault, and its associated temporary editor closed. A Component Library document is then opened in its associated temporary editor (for direct editing), presenting the following:

  • Definitions for all components that are associated to (reference) the Symbol Item.
  • The Model Links region shows the latest (just released) revision for that Symbol Item.
  • The entry for the linked model - in the applicable Models field of each component definition - is set to use that latest revision of the just-released Symbol Item.
When multiple Component Items use the Symbol Item, rather than separate instances of Component Libraries being opened, a single CmpLib document presents a merged view of the world, with all parameters and model links - used by the source component definitions - presented.


Example of pushing a change made to a Symbol Item, through to a Component Item that references it.

Unless you need to make any further adjustments, simply click the  button (in the editor's standard toolbar), to release the modified definition(s) into new revision(s) of the corresponding Component Item(s), back in the target vault:

  • If only a single Component Item is affected, the Create Revision dialog will appear. Change Comment, Description, and add release notes as required. After clicking OK, the release will proceed, and the temporary Component Library editor then closed.
  • If multiple Component Items are affected, the Release Manager dialog will appear. This lists all component Items that are scheduled to be released - by default all enabled for inclusion in the release. Make any changes - to Comment, Description, and inclusion (Enabled option) - as required, then click the Release Items button. View the impending release changes in the subsequent Confirm Release dialog, then click OK. Once the release process completes - indicated by Release Successful in the applicable Action-Status field(s) - close the dialog. The temporary Component Library editor will also then be closed.

Downloading Released Data

Download the data stored in a revision of a Symbol Item by right-clicking on that revision 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 name. The file can be found in the Released folder therein.

Access the Download command from the top-level entry for a Symbol Item itself, to download the schematic library file 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.

Migrating Existing Schematic Libraries

Main page: Streamlined Migration of Existing Libraries to an Altium Vault

Altium Designer, in conjunction with Altium Vault (3.0 or later) provides a streamlined, simple process to quickly migrate your existing libraries to an Altium Vault. The GUI to this process - the Library Migrator view - presents an intuitive flow that takes initial selected libraries, and migrates them to a target Altium Vault. 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 set of vault components, and the many benefits that such components enjoy (high-integrity, lifecycle management, centralized storage and management, where-used functionality, ease of design resuse). And while the migration process can be configured - giving you enhanced control over how that migration is performed - at its most simplistic, you can simply accept the default settings and set the migration in motion within a matter of clicks.

All information that is present in an original source library is migrated, in order to arrive at a folder of unified components (vault components that have assigned part choices), with all referenced domain models (schematic symbols, PCB footprints, 3D Models, Simulation Models), and parametric information. Component templates can even be created, and used to create those vault components. And if your original components have multiple PCB footprints defined, you can rest assured that the Library Migrator will bring those models across, and keep the current default footprint too.


Accessing the Library Migrator view - the 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 vault 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 vault 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.

 

Batch Releasing File-based Schematic Libraries

If you have a set of file-based schematic libraries (*.SchLib) 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 symbols stored across multiple source documents, in a nominated source folder location.

The Release Manager is considered to be a legacy tool. It is highly recommended to use the Library Migrator when migrating your existing component libraries into an Altium Vault.

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


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

Setting up for release couldn't be simpler:

  • Set the Document Type to SCHLIB.
  • Point to a top-level folder containing the schematic library files 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 library file.
  • Use the Default Options for New Released Symbols 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 SYM-{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 library files 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 symbols that you want to release and then click the Prepare Items and Documents button to effectively commit the link information to the source schematic library files involved in the release. Once saved, proceed with the release by clicking the Release Items button.

The Release Manager provides tools which aid in the migration of components stored in schematic component libraries. These include a splitter, for splitting the active SCHLIB into separate libraries containing a single schematic component respectively, and a tool for generating Component Libraries automatically from the active source schematic library.

 

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

お問合せ

お近くの営業所にお問合せください。

You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 無償評価版
Altium Designer 無償評価版
Altium Designerを使用していますか?

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

評価版ライセンスが必要な理由を下記から選択してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

その場合、評価版ライセンスは不要です。

ボタンをクリックして、最新のAltium Designerインストーラをダウンロードしてください。

Altium Designerインストーラをダウンロードする

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

Altium Designerの新規ライセンスのお見積もりをご希望の場合、下記のフォームに入力してください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

Altium Designerサブスクリプションをご利用中の場合、評価版ライセンスは不要です。

お客様がAltium Designerサブスクリプションの有効なメンバーではない場合、下記のフォームに入力して無償評価版をダウンロードしてください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

Altium Designerを評価する理由を下記から選択してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

無償評価版を使用するには、下記のフォームに入力してください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

アルティウムでは、学生の方や教育機関を対象とした特別価格ライセンスを提供しています。アカデミックライセンスの詳細については、こちらをクリック してください。.

また、下記のフォームに入力して無償評価版をリクエストしていただくことも可能です。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

その場合、Altium Designerビューワーの無償ライセンス(有効期間6か月)をダウンロードできます。

下記のフォームに入力してライセンスをリクエストしてください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。

素晴らしいですね。アルティウムではモノづくりに最適なプログラムを提供しています。

Upverterは、コミュニティ主導型の無償プラットフォームで、お客様のような作り手の要求に合わせて設計されています。

試してみる場合、こちらをクリック してください。

弊社の営業担当より詳細情報をご案内しますので、アルティウムジャパン までお問い合わせください。.
Copyright © 2019 Altium Limited

その場合、Altium Designerビューワーの無償ライセンス(有効期間6か月)をダウンロードできます。

下記のフォームに入力してライセンスをリクエストしてください。

プライバシーポリシーに同意の上、[ダウンロード]をクリックしてください。ご登録いただきましたメールアドレスにメールマガジンが送信されます。メール配信の停止は、メール内の​通知設定​​でお手続きいただけます。