Plane Design Rule Types Available for PCB Layout in Altium Designer

The design rules of the Plane category are described below.

The Plane category of design rules.

Power Plane Connect Style

Default Rule: required i

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

Constraints

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 of the copper ring around the hole, measured from the edge of the hole to the edge of the air gap.

Rule Application

During output generation.

Notes

• 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.

Power Plane Clearance

Default Rule: required i

This rule specifies the radial clearance created around vias and pads that pass through but are not connected to a power plane.

Constraints

Default constraints for the Power Plane Clearance Rule

Clearance - the value for the radial clearance.

Rule Application

During output generation.

Polygon Connect Style

Default Rule: required i

This rule specifies the style of the connection from a component pad, or routed via, to a polygon plane.

Constraints

Default constraints for the Polygon 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 polygon pour, as present in previous versions of the software.
  • Advanced - in this mode, you have the ability to separately define thermal connections for thru-hole pads, SMD pads, and vias, respectively.
• 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 polygon 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 polygon plane.

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

• Air Gap Width - the distance between the edge of the pad/via and the surrounding polygon. Note that this constraint is also applied when using the No Connect style.
• Conductor Width - how wide the thermal relief copper connections are.
• Conductors - select the number of thermal relief copper connections:
  • 2 - two conductors at the chosen Rotation angle.
  • 4 - four conductors at the chosen Rotation angle.
  • Auto - the software will define one thermal relief conductor from the center of each separate edge of the pad/via shape, radiating outward at 90° to that edge of the shape (with one conductor for every 90° of arc in a rounded shape). For pads, Auto mode maintains this pad edge-to-thermal conductor relationship regardless of the pad rotation (the spokes rotate with the pad). Note that this is not true for vias, as they do not have a discrete rotation setting.

  • Min Distance - the Min Distance option can also be enabled to specify the minimum distance allowed between any two adjacent thermal relief conductors (as measured along the edge of the shape). If adjacent thermal relief conductors are located closer than Min Distance, sufficient thermal conductors are removed to ensure that the Min Distance setting is achieved between all adjacent thermal relief conductors. 

    Additional thermal relief connections can be defined if required, and their location can be tailored to suit the design requirements. Learn more about Defining Custom Thermal Reliefs. 

• Rotation - the angle of the copper connections when the 2 or 4 Conductor mode is selected.

Rule Application

During polygon pour.

Notes

• 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.