Pad & Via Templates and Libraries

Along with Track objects, Pads and Vias are fundamental elements of all circuit board designs that are effectively placed and configured as custom objects in each PCB layout. The need for design reuse and the standardization of Pad & Via properties, to date, has been managed by ad hoc guidelines and appropriate design rules as each pad or via is placed.

To raise the design reuse and management capabilities for Pads and Vias in PCB designs to a new level, Altium Designer has introduced automated Pad and Via templates, Pad and Via template Libraries, and a number of associated Pad and Via management Panels.

The concept of Pad and Via templates that can be collected in a Library is not unlike that of PCB footprint Libraries, although somewhat more basic. The templates are composed of primitive design elements with defined properties, and these can populate an associated library. In turn, this saved library can be reloaded and used to place instances of predefined Pads and Vias in any PCB design (or PCB Library). However, note that there are a few unique aspects of Pad & Via templates and libraries, and the way they are managed.

The advanced Pad and Via Template features in Altium Designer include:

• Pad and Via Templates – configuration definitions for Pads and Vias.
• PCB Pad Via Templates Panel –  a panel dedicated to managing  both ‘local’ and Library based Pad/Via templates.
• Pad Via Libraries – collections of Pad and Via templates stored as a *.PvLib file.
• Pad Via Library Panel – the library panel associated with the Pad/Via Template Editor.
• Pad/Via Template Editor – an editor pane used to create and edit Pad/Via template definitions.
• PCB Panel Pad & Via Template mode – a specialized PCB panel mode for managing Pad and Vias in a board design, and the relationship to their associated templates.

Pad and Via Templates

Pad and Via Templates store the base configuration of a Pad Via, including its size, shape, padstack type, Paste/Solder Mask and Hole information, and so on. The configurations are automatically named in compliance with IPC standards (specifically, the IPC-7251/7351 Padstack naming conventions) and are used to define Pad and Vias placed in a PCB design file.

Pads and Via types that are present in an existing PCB design are automatically named in this way when the design file is opened, ensuring compliance with the new functionality. To observe this behavior, inspect the properties of an existing Pad or Via from its associated Properties dialog – double click on the object, or select the object then choose Properties from the right-click context menu.

The auto-generated Pad or Via template name shown in the properties dialog.

Note the assigned Template name in the dialog’s Pad/Via Template section. In line with the IPC guidelines the name is derived from the base Pad/Via properties such as its dimensions, shape, hole and Paste/Solder mask configuration. If those properties are changed, the template name will change to reflect the new configuration.

The IPC naming system is metric based where one unit is equivalent to one hundredth of a millimeter (10^-5 meters, 10µm), so for example, the template for a 1.5mm circular pad with a 0.8mm hole is named c150h80 – where c indicates circular (round) and h prefixes the hole size.  Further letter/integer combinations are added for specified Paste/Solder Mask properties.

All pad and via types in the current PCB document are configured as ‘local’ Pad/Via templates, and any one of these can be selected as an alternative from the Template name drop-down menu in the in the Pad/Via properties dialog.

The Template name drop-down menu allows the template to be changed for the current Pad or Via.

Note that the Pad/Via Template section in the dialog also provides a Library link area. This will show <Local> for a pad/via that is within the current PCB file – a ‘local’ template – or include a Library reference if the template has been sourced from a Pad Via Library (see below).

PCB Pad Via Templates Panel

The PCB Pad Via Templates panel is a specialized panel that lists the pad/via templates that are assigned to the current PCB document (Local), or those available from Pad Via Libraries that have been installed or included within the current design project (Available libraries).

Open the panel from the workspace status bar (bottom right of the editor area) by selecting PCB » PCB Pad Via Templates.

The panel provides the dual function of accessing both local and library based Templates.

The two library concepts presented in the panel can be summarized as:

• Available Pad and Via Libraries – Loaded or installed Pad Via Libraries (file-based collections of Pad/Via templates). The upper section of the panel lists templates contained in the currently selected Pad Via Library.
• Local Pad/Via Library – The collective term for Pad/Via Templates that are used for the current board design, including any that have been sourced or added from a Pad Via Library. The lower section of the panel list templates that apply to the current board design.

Local Pad & Via Library

The entries listed in the lower Local Pad & Via Library section of the panel represent the pad/via configurations (templates) assigned to the current board design. A preview of the selected template is shown at the bottom of the section.

The templates listed here represent Pads and Vias saved within the PCB file, and are not contained in a separately defined 'library' as such. A selected template can be reused in the current board as a new pad or via instance by dragging it onto the layout, or by selecting Place from its right-click context menu.

Placing a local Pad template instance.

Since template names listed in the Local Library are derived from Pads and Vias in the current PCB layout, if all instances of a particular pad/via configuration have been deleted from the board, its corresponding template will be removed from the Local List.

However, if a placed Pad or Via has been sourced from a Pad Via Library, its template will be retained in the Local list when all instances of that pad/via have been deleted from the board – or changed to a different template type. Instances of Pad Via Library templates that are no longer required can be removed from the local ‘database’ record with the Remove Unused Pad/Via button.

Pad & Via Template Libraries

The upper section of the panel, Available Pad/Via template Libraries, applies to the templates contained in the selected Pad Via Library – see below for more information. Templates from the selected library can be applied to the PCB by dragging, or via the right-click menu, as outlined above.

The contents of a selected Pad Via Library file.

As with similar library panels, the current library file can be selected from the Library name drop down menu list, and a Library’s contents navigated through the associated Filter field.

Pad Via Library Template to Local

Library based Pad/Via templates can also be added directly to the Local library list by right-clicking on the template name and selecting Add to Internal Library from the context menu, or by simply dragging the template from the panel’s Pad/Via library section to a blank area the Local library section.

This is equivalent to placing a pad/via sourced from Pad Via Library template, then deleting it from the board – thereby registering that template as locally available.  To replace a local template, rather than add one to the local list, see Replace a Local Template further below.

A Pad Via Library Template added to the Local library becomes available for configuring project design options.

Pad Via Library sourced templates that are available to the local document can be applied to Rules, configurations and defaults for the current project. When placing Via Stitching for example, the placed via characteristics are defined by the template selected in the Add Stitching to Net dialog – Tools » Via Stitching/Shielding » Add Stitching to Net.

Local Pad/Via templates sourced from a Pad Via Library become available for configuration options.

Replace a Local Template

A library based Pad/Via template can also replace a Local template, which will update Pads or Vias on the board that use the (local) template.

To do so, drag the desired library template from the Pad/Via Library section of the panel to the Local Pad & Via Library section of panel, but in this case, drop the library template on top of the existing local template entry. Any instances of free or component pads/vias that use the template will be updated to the new library template style.

In the below animated image, note that the design's C4 and C5 component pads physically change to the type determined by the 'dropped' library template – from r32_36 to r30_50, as also indicated by the Local library list.

Drop a library template on top of a local template entry to replace it for all instances in the design.

Update from Pad Via Library

The Update button in the PCB Pad Via Templates panel's Local section provides a method to update the Pad or Vias templates in the current design from their source.

For example, in the case of a Pad that has been placed from a Pad Via Library template and the source Library template has been subsequently updated, the Update function will pull in those template changes to the PCB – thereby updating all Pads that use the Library template.

The template update is configured by the Update Pad or Via dialog that opens when an update is instigated. This lists the details of the detected change(s) that will be applied.

Pad/Via Templates that are detected as differing to their source library version can be updated from the Library to the PCB design.

Three update options are offered by the dialog to control the update process:

• Update locked objects – this will force a Pad/Via object’s template to be updated, regardless of its Locked status.
• Update free objects – update only Pad/Via templates that apply to free Pads and Vias.
• Update component objects – update only Pad/Via templates that apply to the Pads and Vias used in components.

This synchronization behavior is established by the Library link property of Pad and Vias, as seen in the Pad/Via properties dialog. An indication that differences exist between the local version of the template and the source template is provided in the Changed column of the Pads/Vias section in the Pad & Via Templates mode of the PCB panel – see below.

Loading a Pad Via Library

An existing Pad Via Library is added to the project or Installed by clicking on the button to the right of the panel's Library name selector menu, which opens the Available Libraries dialog.

Use the Installed tab option to load an existing library (*.PvLib) that will be available for all projects, and the Project tab to add an existing library to the current project. See below for information on creating a Pad Via Library.

Install an external Pad Via Library, or use the Project tab to add an existing library to the current project.

Pad Via Library

An existing Pad Via Library can be added to a design project as mentioned above, or a new library can be created by selecting File » New » Library » Pad Via Library from the main menu – or by right-clicking on the current project and selecting Add New to Project » Pad Via Library from the context menu.

A new Pad Via Library is automatically added to the current project in the Libraries – Pad Via Library Documents sub folder. With the new library active, the Pad Via Library Editor window is also opened in the main workspace (initially blank), and the Pad Via Library panel becomes active.

Pad Via Libraries are managed by the Pad Via Library panel, and their constituent Templates are edited with the Pad /ViaTemplate Editor.

Pad Via Library Panel

The Pad Via Library panel lists the Pad and Via templates contained in the current library. The preferred units are selected from the Display Units drop down menu.

To create a new Pad or Via template, right click within the panel and select Add Pad Template or Add Via Template (respectively) from the associated context menu. Use Delete to remove a template from the Library.

The panel provides access to Templates contained in the current Pad Via Library. Right-click to add a new Template.

Pad/Via Template Editor

The Pad/Via Template Editor provides the base configuration options for a Pad or Via template that can be applied to a Pad or Via in a PCB or PCB Library document. These include the main properties of a Pad/Via configuration, while document-specific properties are (such its position, orientation, layer, etc) are defined when the Pad or Via is placed in a design document.

The editor provides an interactive graphical representation of the Via or Pad padstack.

The majority of Pad/Via configuration options are standard and familiar Altium Designer Pad and Via settings (Size, Hole and Mask, etc), and the padstack option is defined in broad terms for Pad templates – SMT (single layer) or Through Hole.

A graphical representation of the current Pad or Via configuration is also shown in the lower section of the Editor pane. This provides a physical preview of the shape and layer attributes of the current Pad/Via.

Note that the current Pad/Via template Name can be changed from the auto-generated IPC version to a custom name – conversely, the name can be reset to the IPC compliant version by clicking the associated button. When a custom named Library template is applied to a Pad/Via placed in a PCB document, the name is persistent until the link to the library is intentionally broken.

Editing a placed Library Template Pad/Via

In practice, when Pad or Via is placed in a PCB from a Library template, usually from the PCB Pad/Via Templates panel, it will exhibit a large number of parameters that can’t be edited. These correspond to the parameters that are defined in the template, and as a result, they are locked as read-only (as illustrated in the below image) until the pad or via is unlinked from the library template.

Parameters defined by the applied Library Pad/Via template are read-only, here shown highlighted in gray.

The pad/via can be unlinked from the library template by clicking the Unlink control, which frees the locked parameters for editing and reverts the pad/via name to the auto-generated IPC standard format.

PCB Panel Pad & Via Templates mode

To provide advanced control of the Pad and Via templates used in the current PCB document, Altium Designer’s PCB Panel provides dedicated Pad & Via Templates mode. This mode can be accessed from the mode drop-down menu at the top of the PCB panel.

The Pad & Via Templates mode in the PCB panel behaves in a similar way to other panels modes, with a hierarchical filtering action applied to lower order panel sections.

The panel’s Pad & Via Templates mode provides a hierarchical view of Template application in the active PCB design document, and is divided into three descendant sections:

• Libraries
• Templates
• Pads/Vias

Libraries section

This list shows the Pad & Via template instances in the design as a collection of virtual and physical libraries.  Theses filter the templates included in the lower panel section list, and are arranged as:

• All – show all Pad and Via templates, including those used from Pad & Via Libraries.
• Pads – show all Pads, both local and library based.
• Vias – show all Vias, both local and library based.
• Local – show all Pads and Via templates applied to the board, but not those added from Pad Via Libraries.
• Pad & Via Libraries – only show Pad and Vias templates that have been applied from the selected Pad Via Library.

Templates section

This panel section provides a list of all Pad/Via templates that are used in the current PCB design. Its columns include the template source Library (local or Pad Via Library name) and the number of Pad/Via instances for each template (Count).

Any number of the listed templates can be saved to a separate Pad Via Library. To do so, select multiple templates using standard Shift+click and Ctrl+click techniques and click the Save as Library button. The Library will be automatically added to the project, and be can be saved as the desired *.PvLib file name using File » Save As from the Projects panel.

The Templates section also allows a Pad Via Library based template to be placed in the PCB design with the Place button. Select the desired Pad Via Library in the top Libraries section of the panel to enable this capability.

Pad/Via section

The Pad/Via list section of panel is populated with the individual Pad/Via instances of the template selected in the above Templates section.

As each Pad/Via instance is selected, the object is graphically highlighted in the editor workspace, as defined by the panel’s standard highlight, zoom and selection options – located in the very top portion of the PCB panel.

Each listed instance in the Pads/Via panel section is accompanied by a Changed indicator box, which becomes checked when a linked Library source template differs from that used in the local Pad or Via. In other words, when the source Pad Via Library has been updated.  The Changed indicator will also become checked if the local Pad/Via has its padstack type changed – say a Pad instance is locally changed from Multilayer to Single layer.

In all cases, the local version of the Pad or Via can be updated (or reverted) to the current template in the source Pad Via Library using the PCB Pad Via Templates panel Update button, as outlined above.

Routing Vias Rule

A new Template Preferred constraint option has been added to the RoutingVias rule definition, which can be selected as an alternative to the familiar Min/Max Preferred constraint. As the name implies, this option uses selected Via templates for the Via placement constraints during Interactive Routing.

To configure this option, select Design » Rules then navigate to the Design Rules – Routing – Routing Via Style and select Template Preferred as the constraint option in the PCB Rules and Constraints Editor dialog. The available template options for the mode are defined by the Pad Via Library templates present in the Local Library – those that have been placed in the board design, or manually added to the Local Library.

Within the templates list, check the Enable box for templates you would like to be available for placement during Interactive Routing, then click OK to accept the changes and dismiss the dialog.

In the same way as when using the alternative Min/Max Preferred rule constraints during Interactive Routing, when a routing Via is placed (2 or + key) you can cycle through the available Via options (4 key). In this case, the options will toggle through the Via templates that have been enabled in the RoutingVias rule Template Preferred definition list.

The placed Via type can also be selected from the enabled Template drop down list in the Interactive Routing for Net dialog (press Tab during Via placement).