Working with the Power Plane Connect Style Design Rule on a PCB in Altium Designer

This document is no longer available beyond version 21. Information can now be found here: Power Plane Connect Style Rule for version 24


Rule category: Plane

Rule classification: Unary


This rule specifies the style of the connection from a component pin to a power plane.

All design rules are created and managed within the PCB Rules and Constraints Editor dialog. For a high-level view of working with the design rules system, see Defining, Scoping & Managing PCB Design Rules.


Default constraints for the Power Plane Connect Style rule. Roll the mouse over the image to compare the two modes of operation available.Default constraints for the Power Plane Connect Style rule. Roll the mouse over the image to compare the two modes of operation available.

  • Mode of Operation - the rule can operate in one of the following two modes:
    • Simple - this mode is the generic setting for how pads/vias connect to a power plane, as present in previous versions of the software.
    • Advanced - in this mode, you have the ability to define specific thermal connections for pads and vias, separately.
  • Connect Style - defines the style of the connection from a pin of a component, targeted by the scope (Full Query) of the rule, to a power plane. The following three styles are available:
    • Relief Connect - connect using a thermal relief connection.
    • Direct Connect - connect using solid copper to the pin.
    • No Connect - do not connect a component pin to the power plane.

The following constraints apply only when using the Relief Connect style:

  • Conductors - the number of thermal relief copper connections (2 or 4).
  • Conductor Width - how wide the thermal relief copper connections are.
  • Air-Gap - the width of each air gap in the relief connection.
  • Expansion - the radial width measured from the edge of the hole to the edge of the air gap.

How Duplicate Rule Contentions are Resolved

All rules are resolved by the priority setting. The system goes through the rules from highest to lowest priority and picks the first one whose scope expression matches the object(s) being checked.

Rule Application

During output generation.


  • The Simple mode is the default mode, for a newly created rule of this type.
  • After setting and applying constraints in Advanced mode, be aware that switching back to Simple mode is considered a modification - clicking Apply or OK will effect the simple definition, overriding the individual advanced definitions specified previously.
  • Power planes are constructed in the negative in the PCB Editor, so a primitive placed on a power plane layer creates a void in the copper.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

Набор доступных функций зависит от вашего уровня доступа к продуктам Altium. Ознакомьтесь с функциями, включенными в различные уровни Подписки на ПО Altium, и функциональными возможностями приложений, предоставляемых платформой Altium 365.

Если вы не видите в своем ПО функцию, описанную здесь, свяжитесь с отделом продаж Altium, чтобы узнать больше.