Altium Designer Documentation

Managed 3D Models in an Altium Vault

Modified by Jason Howie on Jul 31, 2017

Parent page: Vault Items

Altium Designer, in conjunction with Altium Vault, caters for the ability to create and manage 3D models. Used in a similar fashion to file-based linked 3D models,  a vault-based 3D Model Item can hold a 3D model file, that is then referenced through a 3D body attached to a standard 2D footprint. Once a 3D Model Item has been created (and data uploaded 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.

Folder Type

When creating the folder in which to store a 3D Model Item, you can specify the folder's type. This has no bearing on the content of the folder - uploading will always result in a 3D Model 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 3D Model Items, set its Folder Type as 3D Models, 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 (A3DL - Altium 3D Library) or the content type (A3D - Altium 3D):

  • $CONTENT_TYPE_CODE-001-{0000} - for example, A3D-001-0001.
  • $CONTENT_TYPE_CODE-001-{A00} - for example, A3D-001-A01.
  • $FOLDER_TYPE_CODE-001-{0000} - for example, A3DL-001-0001.
  • $FOLDER_TYPE_CODE-001-{A000} - for example, A3DL-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 3D Model 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. STEP3D-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 the target 3D Model Item in which to store your 3D model file, ensure that its Content Type is set to 3D Model, in the Item Properties dialog. If you are creating the Item in a 3D Models type folder, this Item type will be available from the right-click context menu when creating the Item.


Creating a 3D Model Item within a 3D Models folder - the correct Content Type is available on the context menu.

When defining the 3D Model Item, to which the source 3D model file is uploaded, 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 3D Model Item are: Basic Lifecycle and 1-Level Revision Scheme, respectively.

Once a 3D model file has been uploaded into the initial revision of a 3D Model 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 3D Model 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 3D Model Item offers.

Uploading a 3D Model File

So far, we've discussed the support for a 3D Model Item in the vault, in terms of related folder and item types. Uploading an 3D model file into the revision of such an item can be performed in a couple of ways.

Upload Menu

A 3D model file can be uploaded by right-clicking on the required 3D Model Item in the Vaults panel, and choosing the Upload command from the context menu. The standard Windows Open dialog will appear. Browse to, and open, the required model file. Supported formats are:

  • STEP File (*.step; *.stp)
  • Parasolid File (*.x_t; *.x_b)
  • SolidWorks Part File (*.sldprt)
If the Item has no planned revision, upload will be to the next planned revision, created on-the-fly as part of the upload process.


Manually specifying the 3D model file to be uploaded to the target 3D Model Item.

Once the desired file is selected, proceed with the upload by clicking the Open button. The graphical depiction of the uploaded model can be viewed in the Preview aspect view for the Item Revision, in the Vaults panel.


The graphical depiction of the uploaded model can be viewed in the Preview aspect view for the Item Revision.

Drag and Drop from Windows Explorer

A 3D model file can also be uploaded by dragging the selected file from a source folder in your Windows Explorer, and dropping onto the required target 3D Model Item in the Vaults panel.

If you attempt to drag and drop more than one 3D Model file, the Release Manager dialog will automatically launch. Use this to complete upload of multiple models.

The Release File dialog will appear, with the dragged file listed in the Sources area. Add a Comment, Description, and any Release Notes as required, and then click the OK button.


Uploading a 3D model using the drag and drop method.

If the existing 3D Model Item has no planned revision, upload will be to the next planned revision, created on-the-fly as part of the upload process. If the 3D Models folder has no pre-created 3D Model Items, a new 3D Model Item (and planned revision) will be created, as part of the upload process. Initial naming of the new Item will be in accordance with the Item Naming scheme defined at the folder level. If the folder has no naming scheme defined, naming will follow the $CONTENT_TYPE_CODE-001-{0000} scheme.

Reusing a Managed 3D Model Item

Related page: Controlling Access to Vault Content

Once a 3D model file has been uploaded 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 3D model can be reused in future board-level design projects.

A 3D body is used to provide the three-dimensional representation of the component in the PCB domain, and is typically placed and defined in conjunction with the standard 2D footprint model, when defining a footprint model (which is then released to the vault as a revision of a target Footprint Item).

The quickest, and easiest way to use a revision of a 3D Model Item, is to place it directly from the vault into a PCB or PCB Library document, creating a 3D Body object that references that Item Revision. The 3D Body object can then be fine-tuned as required. To place:

  • Ensure a PCB Library (or PCB) document is open as the active design document.
  • Either right-click on the required revision of the 3D Model Item and choose the Place command from the context menu or, even faster, click on the revision, then drag and drop it onto the document.
Right-click and Place (or drag and drop) the top-level entry for an Item itself, to place an instance of the latest revision of that Item.

Conversely, if you are defining the 3D Body object, and want to reference a 3D model that is stored in an Altium Vault, this can be done from within the 3D Body dialog, when defining the properties for the body.

To do so:

  1. Set the 3D Model Type to Generic 3D Model.
  2. In the Generic 3D Model region of the dialog, choose the Vault option.
  3. Click the Choose button to the right of the Item Revision field. This gives access to the Choose Item dialog - essentially a trimmed incarnation of the Vaults panel. Use this dialog to browse to, and select, the revision of the required 3D Model Item. After clicking OK, a link will be created between the 3D Body and the target revision of the 3D Model Item. Evidence of this link can be seen back in the 3D Body dialog.


Manually linking the 3D Body object to a revision of a 3D Model Item, in the target vault.

The 3D Model Item being used can be changed at any time - simply click Choose and select a revision of a different 3D Model Item.
The status of the linked 3D Model Item is reflected in the 3D Body dialog. If a newer revision of the linked Item is available, simply click the Update to latest button, to use that latest revision.

Releasing a PCB 2D/3D Component Model into the Vault

When directly editing the source 2D footprint model stored within a revision of a Footprint Item - within a temporary PCB Library Editor - you can define a 3D Body object for it, with that body referencing (linked to) a revision of a 3D Model Item in an Altium Vault. The following happens upon release of that footprint model:

  • The 3D Model link is detected and the revision of the 3D Model Item will appear listed as a child Item of the Footprint Item, in its Children aspect view.
  • The revision of the 3D Model Item is detected as 'being used' and will therefore list the parent Footprint Item in its Where-used aspect view.

Updating a 3D Model Item

If you need to change the 3D model stored in a 3D Model Item, simply upload the required new model to that Item - the new model will be stored in the next revision of that Item.

Updating Related Footprint Items

When you make a change to a 3D model, the moment you upload that change into a new revision of the 3D Model Item, any Footprint 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 footprints, with the respective model links updated to use the latest revision available. To streamline this process, Altium Vault, in conjunction with Altium Designer, facilitates the ability to update related Footprint Items - at the point of uploading to the latest revision of the 3D Model Item.

Once uploaded, if any Footprint Items currently reference the Item, a dialog will appear asking whether or not you wish to update those items.

If you want to keep all related Footprint Items using the current revision of the 3D Model Item, simply click No in the dialog. Only the model itself will then be uploaded.

A PCB Library document is then opened in its associated temporary editor (for direct editing). When multiple Footprint Items use the 3D Model Item, rather than separate instances of PCB Libraries being opened, a single PcbLib document is presented, containing all affected PCB 2D/3D component models.

The revision of the referenced 3D Model Item is not updated to the latest automatically - you will need to do this manually, if required, from the 3D Body dialog.

Once the 3D body for a model is updated to reference the latest revision of the 3D Model Item (where needed), simply click the  button (in the editor's standard toolbar), to release the modified model(s) into new revision(s) of the corresponding Footprint Item(s), back in the target vault:

  • If only a single Footprint 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 PCB Library editor then closed.
  • If multiple Footprint Items are affected, the Release Manager dialog will appear. This lists all Footprint 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 PCB Library editor will also then be closed.
As part of the re-release of the Footprint Item(s), you will also have the opportunity to update an related Component Items that reference those Items.

Downloading a 3D Model File

Download the 3D model file stored in a revision of a 3D Model Item, by right-clicking on that revision and choosing the Operations » Download command from the context menu. The 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 3D Model Item itself, to download the 3D model 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.

Batch Releasing File-based Models

If you have a set of file-based 3D models (*.stp, *.step, *.x_t, *.x_b, *.sldprt) 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 models 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.


Batch-release 3D model files using the Release Manager.

Setting up for release couldn't be simpler:

  • Set the Document Type to 3DModel.
  • Point to a top-level folder containing the 3D model 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 3D model file.
  • Use the Default Options for New Released 3D Models 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 3DModel-{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 3D model 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 3D models that you want to release and then click the Prepare Items and Documents button to effectively commit the link information to the source 3D model files involved in the release. Once saved, proceed with the release by clicking the Release Items button.

The 3D model filename will be used as that uploaded model Item's Comment.

3D Model Extraction

Where 3D models (e.g. STEP) have been embedded into the 2D footprint models within a PCB Library document (*.PcbLib), the Release Manager provides a neat little utility with which to extract those models. To do so:

  1. Launch the Release Manager (File » Release Manager).
  2. Set the Document Type to PCBLIB.
  3. Point to a top-level folder containing the PCB Library(ies) you want to extract 3D models from. Files can be stored in sub-folders within this folder.
  4. Leave the Default Options for New Released PCB Components at their defaults - you are not actually going to release the PCB Library footprint models.
  5. Hit the Analyze Folders button - this loads the PcbLibs.
  6. Click the Migration Tools button and choose Extract 3D Models from the menu.
  7. In the Generate 3D Model Files dialog that appears, use the Options region to determine file generation. Firstly, specify where the generated files are to be stored - either in a sub-folder of the location in which the source PCB Library resides, or in a specified folder elsewhere. By default, a sub-folder named Models3D will be created. Change this naming to something more suitable as required. If the nominated folder exists, it will be used. If not, it will be created.
  8. Optionally choose to Overwrite existing files - have existing 3D model files with the same name overwritten when new files are generated.
  9. After defining options as required, click OK. Generation will proceed and a confirmation dialog will appear when the process is complete, stating how many 3D model files were generated.
Each 3D model file is named using the name of the 2D footprint model.
Only embedded 3D models can be extracted (not extruded, cylinder, or sphere).


Example 3D model files generated from a PCB Library by using the extraction tool.

 

If you'd like to comment on the content on this page, use the Ctrl+Enter keyboard shortcut to send us your feedback. To include a section of the page in your comment (a typo, missing/wrong info, or incorrect imagery), highlight the text (max. 200 chars) and/or image first. Please restrict your feedback to documentation issues - for technical assistance refer to the Altium Forums.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text and/or image within the active document:
Request Free Trial

Complete this form to request a free 15 day trial of Altium Designer: