Contact our corporate or local offices directly.
Along with Track objects, Pads and Vias are fundamental elements of all circuit board designs. Each Pad and Via can be configured as a custom object during or after placement.
To raise the design reuse and management capabilities for Pads and Vias in PCB designs, Altium Designer also supports: automated Pad and Via template creation; 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 Pad Via Template library does not store actual Pads and Vias, rather it stores pre-configured definitions that are applied to an instance of a Pad or Via as it is placed. Saved Pad Via Template libraries can be loaded and used to place instances of predefined Pads and Vias in any PCB design or PCB footprint library.
For each unique Pad or Via placed into a board design, a Pad/Via Template is automatically created, named and stored in the board file. The Template stores the base configuration of the Pad/Via, including its size, shape, padstack type, Paste/Solder Mask and Hole information, and so on. The configuration is automatically named in compliance with IPC standards (specifically, the IPC-7251/7351 Padstack naming conventions). Every Pad and Via used in the design references its Template, this can be seen in the Properties panel, as shown below.
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. A pad named
r155_125 is a rectangular surface mount pad, of size 1.55mm x 1.25mm; and a pad named
s160h100 is a square, thruhole pad, of size 1.6mm, with a 1.0mm hole. Further letter/integer combinations are added for specified Paste/Solder Mask properties.
To observe this behavior, inspect the properties of an existing Pad or Via from its associated Properties panel by double-clicking on the object or selecting the object then choosing Properties from the right-click context menu.
Panel page: PCB - Pad & Via Templates
Each time a uniquely sized Pad or Via is placed into a PCB design using the Place menu or the Active Bar, a new Pad/Via Template is automatically created in the board file. These templates are referred to as
<Local> Templates. For the current PCB, the list of all used Pad and Via Templates can be examined in the PCB panel when it is set to the Pad & Via Templates mode.
Use the Pad & Via Templates mode of the PCB panel to locate and select a Pad or Via of interest. Selected Pad(s) or Via(s) can then be edited to use a different template in the Properties panel, choose the required template in the Template dropdown. The PCB panel is also used to save selected Pads and Vias to a Pad Via Template library, more on this in the Creating and Editing a Pad Via Template Library section.
As mentioned, existing templates can be saved into Pad and Via Template libraries, and new templates created. The templates in these libraries are made available for use through the PCB Pad Via Templates panel. Local templates are also listed in the panel, making the panel the central resource for working with Pad and Via template libraries.
Panel page: PCB Pad Via Templates
The PCB Pad Via Templates panel is a specialized panel that lists both the Pad/Via templates stored in 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).
Click the button at the bottom right of the workspace then choose PCB Pad Via Templates to open the panel.
The two library concepts presented in the panel can be summarized as:
The entries listed in the lower Local Pad & Via Library section of the panel represent the pad/via configurations (templates) used and saved in the current board design. A preview of the selected template is shown at the bottom of the section.
The templates listed here are Pad Via templates 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 the panel's right-click context menu.
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 Local 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 removed from the board. 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.
The upper section of the panel, Available Pad/Via template Libraries, is used to work with Pad Via Template file libraries.
A Template can be placed from the selected library into the PCB by dragging from the panel or the right-click context menu. Because the Pad/Via is being placed from an external Template file library, its properties are not available for editing in the PCB, as can be seen in the image of the Properties panel shown below, on the right. To edit the properties of a library-based pad/via its template must be unlinked, more on this in the Unlinking a Template from a Library section.
The drop-down at the top of the panel is used to select which available library is active, in the image below it's the
ExampleViaLib.PvLib. The button is used to open the Available Libraries dialog where Template library files can be added and removed. Available Libraries are discussed below. Use the Filter field to display only templates whose Name starts with that string.
The term Available Libraries means Pad Via Template libraries whose templates are available for use in the current board design. This includes Template libraries that have been added to the current project, and also Template libraries that have been installed in Altium Designer. Both types can be reviewed and managed in the Available Libraries dialog; click the button at the top of the PCB Pad Via Templates panel to open the dialog.
Templates listed in the PCB Pad Via Templates panel can be used in the current board design in the following ways:
PadViaLibraryTemplate = 'r75_140')
PadViaLinkedToTemplate = 'True')
This section discusses the various scenarios where you need to edit Pad or Via templates.
There will be times when you want to apply a different template to existing Pads or Vias (perhaps you're reducing the number of different Vias used in a design). In this situation, use the Pad & Via Templates mode of the PCB panel to locate and select the Pads/Via you want to change. Selected Pad(s) or Via(s) can then be edited to use a different template in the Properties panel by choosing the required template in the Template dropdown.
It is not possible to edit the properties of Pads/Vias using a template from a file-based template library, if it was it would mean that the local instance would no longer match the referenced library template. To edit a Pad or Via that references a library template, the template must be unlinked.
Click the button to unlink a template. When you click this button, a copy of that template is made in the local library, and the selected instance(s) of the Pad/Via are referenced to the local template
If required, a library template can be added to the local library. This can be done by right-clicking on the template name and selecting Add to Internal Library from the context menu, or by dragging the template from the panel’s Pad/Via library section and dropping it in a blank area the Local Pad & Via Library section. Unused Pad/Via library templates can be removed from the local library by clicking the Removed Unused Pad/Via button.
To replace a local template, rather than add one to the local list, see Replace a Local Template below.
If a template for a Pad/Via has been updated in the library and that template has already been used in a board design, click the Update button in the PCB Pad Via Templates panel to update the Pad/Via template in the design. The update will automatically be reflected in all instances of Pads/Vias that use that template in the board.
When an update is instigated, the Update Pads/Vias on Board dialog opens, listing the details of the detected change(s) that will be applied.
Three update options are offered by the dialog to control the update process:
This synchronization behavior is established by the Library property of pads and vias, as seen in the Properties panel when viewing the properties for a selected pad or via respectively. 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.
A library based Pad/Via template can also replace a Local template, which will update the Pads or Vias on the board that use that local template.
To do this, 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. All instances of free or component pads/vias that use the template will be updated to the new library template style.
In the animation below, note that
C2 component Pads physically change to the type determined by the 'dropped' library template – from
Pad Via Template libraries are another design document that can be created in Altium Designer and have the file extension
*.PvLib. Pad Via Template libraries can be included as a project document, and if so, those templates are always available to that project through the PCB Pad Via Templates panel. Template libraries can also be Installed in the panel, making them available to all open projects. Learn more about making templates available in the Working with Pad Via Templates section.
Pad and Via Templates are created and edited by opening a PvLib file. The Pad and Via Templates in the PvLib are listed in the Pad Via Library panel, with the selected Pad or Via Template displayed in the Pad/Via Template Editor, as shown below.
To create a new Template library:
PvLib1.PvLib. At this stage, the file has not been saved to the hard drive; it only exists in the computer memory. Because it is unsaved, the first time you save it, the Save As dialog will open offering to save it to the Default Location defined on the System - Default Locations page of the Preferences dialog.
The Pad Via Library panel lists the Pad and Via templates contained in the current Pad Via Template library. The preferred units for this editing session are selected from the Display Units drop-down menu at the top of the panel.
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 Pad Template Editor is used to configure the base configuration options for a Pad or Via template that can then 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 majority of Pad/Via configuration options are standard and familiar Altium Designer Pad and Via settings (Size, Hole and Mask, etc.). The Pad Template editor shares a common interface design and many of the options with the Via Template editor. Each section of the template editor is described below, with the options that are specific to Pads or Vias marked as such.
Full Stack(for pads this option is available only when the Pad Type is Through hole). Allows pads/vias to have different Size and Shape properties on the layers made available for that mode. Naming element x<Xvalue_Yvalue> added when a different size/shape is defined for the Bottom layer. Naming element z<Xvalue_Yvalue> added when a different size/shape is defined for mid layers.
Contact our corporate or local offices directly.