KB: Applying Polygon Connect Style Rule to Component Pads by Pad Class

Solution Details

Controlling Polygon Connections by Pad Class

Why Use Pad Classes for Polygon Connect Rules

Pad classes are useful when you want to apply consistent polygon connection behavior to a group of pads that may not share the same net but do share a functional or mechanical role. For example, grounding pads for shielding components or thermal vias can be grouped into a pad class and treated uniformly.

Why Polygon Connections May Not Behave as Expected

Altium Designer does not automatically apply polygon connect styles based on pad class unless a specific rule is defined. Without this rule, polygons may connect using default settings, which may not be optimal for grouped pads.

Applying Polygon Connect Styles to Pad Classes

To apply a polygon connect style to pads in a pad class:

• Create a new Polygon Connect Style rule.
• Use a query that targets pads by their pad class.
• Define the desired connection style (e.g., thermal relief, direct connect).

Step-by-Step: How to Apply Polygon Connect Style Rules

1. Open your PCB layout in Altium Designer.
2. Navigate to Design » Rules.
3. In the PCB Rules And Constraints dialog, right-click Polygon Connect Style and choose New Rule.
4. In the Where the Object Matches section, click Query Helper.
5. Enter a query like:
   (IsPad) AND (InPadClass('YourPadClassName'))
6. In the Constraints section, select the desired polygon connection style (e.g., Direct Connect, Relief Connect).
7. Click Apply and OK.
8. Repour polygons to apply the rule.

Note: Under the premise that specific pads should have a certain type of connection, this can be achieved using a Pad Class. Use the PCB editor Object Class Explorer via Design » Classes to create a Pad Class and add the required members. You can then reference the Pad Class in your rule using:
InPadClass('PadClassName')

Additional Notes

• Polygon Connect Style rules apply to both component pads and routed vias.
• Pad classes must be defined before applying the rule. Use the PCB panel » Pad Classes to manage them.
• If multiple rules apply to the same pad, rule priority will determine which one is enforced.
• Object-level overrides can supersede rule-based polygon connection styles.

Further Reading

• Defining, Scoping & Managing PCB Design Rules
• Polygon Connect Style