Drill Pair Reference (New Feature Summary)

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.

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.