Altium Designer Documentation

Drill Pair Reference

Modified by Jason Howie on Apr 11, 2017

A Drill Pair definition in Altium Designer describes a drilled hole’s span between board layers, defined by a Start Layer and a Stop layer. They are used to define the drill hole layer span for Vias such as the default type (top to bottom layer), Blind Vias (a surface layer to an internal copper layer) and Buried Vias (one internal layer to another internal layer).

The application and management of Drill Pairs has been enhanced with the implementation of defined layer combinations based on the board’s layer stack, replacing the approach of nominating individual drill start and end layers when configuring Vias.  Access has also been improved to the Drill-Pair Manager dialog, which is the central location for defining Drill Pairs for the current design.

A Via’s Drill Pair property setting can be accessed from the associated Via dialog as a drop-down list of available Drill Pair configurations, which are predefined in the Drill-Pair Manager dialog.

To set the Drill Pair for that Via, simply select the appropriate drill layer span definition from the dialog’s Drill Pair list.

The dialog also provides direct access to the Drill-Pair Manager dialog, from the button located at the bottom the dialog. The Drill-Pair Manager dialog can also be accessed from the Drill Pairs button in the Layer Stack Manager dialog (Design » Layer Stack Manager).

Drill Pairs are defined in the Drill-Pair Manager dialog through the Drill-Pair Properties dialog, which is accessed by adding a new pair definition or by opening an existing pair’s properties (double-click a pair definition, or click the button).

The Drill Pair start and stop layers can only be selected from those available in the board Layer Stack configuration. Note that the default Drill Pair definition is Top Layer – Bottom Layer.

Drill Pair definitions are consistent across all Via access methods, including Via Stitching and Via Shielding, and the List panels (PCB List, PCBLIB List), Inspector panels (PCB Inspector, PCBLIB Inspector) and PCB panel.

Altium Designer also caters for changed Layer Stack or Drill Pair definitions that may contradict the Drill Pair definition applied to an existing Via.

If for example a Via’s existing Drill Pair assignment is no longer an available option – say, it has been removed from the Drill Pair Manager dialog's definitions – the assigned Drill Pair will be highlighted in red in the Via dialog.

A level of protection is also provided in the situation where a Via’s assigned Drill Pair refers to a layer that no longer exists in the board layer stack. In this case, the Via will revert back to the default Top-Bottom Drill Pair configuration when it is accessed – that is, when the Via itself is selected or it is remotely selected in a List panel, the PCB panel’s Pad & Via Template mode, etc.

Targeting a Drill Pair from a Design Rule

Previously, a design rule could be scoped to target a drill pair using the StartLayer and StopLayer query keywords. With the introduction of definable drill pairs, this is now done using the DrillPair keyword, using the following syntax:

DrillPair = '<UpperLayerName> - <LowerLayerName>'

for example:

DrillPair = 'TopLayer - SignalLayer1' - note that the layer names are written as they are entered into the Layer Stack Manager dialog.

 

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: