In PCB design, copper pour is an efficient way to utilize board space and improve electrical performance. Copper pour, also known as copper flooding, involves filling unused areas of the PCB with copper to create a continuous reference plane. The primary benefits of copper pour include reducing ground impedance, enhancing interference resistance, lowering voltage drops, increasing power efficiency, and minimizing loop area by connecting to the ground plane, which also improves electromagnetic compatibility (EMC).

Today, we’ll share some practical tips for designing copper pour in Altium Designer to help you achieve more efficient, professional PCB designs. Here are some valuable methods:

Setting Different Clearances for Copper Pour and General Clearance

In PCB design, the overall clearance and copper pour clearance may need to differ. For instance, the spacing between copper pour and other components or traces may need to be greater to reduce electromagnetic interference. Here’s how to set it up:

  1. Quick Access to Rules Editor: Use the shortcut “D” + “R” to open the PCB Rules and Constraints Editor.

  2. Create a New Rule: Right-click on Clearance and select New Rule.

  3. Set General Clearance: For example, set the general clearance to 6 mil (0.152mm) and name this rule Clearance.

  4. Set Copper Pour Clearance: Create a new rule with a copper pour clearance of 0.5mm and name it Polygon. Follow these steps:

    • In the Where The First Object Matches window, select Advanced (Query) and click Query Helper….

    • In the Query Helper window, type “inp…” to auto-select InPolygon, then click OK.

Setting Copper-to-Board Edge Distance Different from Copper Pour Clearance

The distance from the copper pour to the board edge might need to differ from the general copper pour clearance to avoid short circuits or other risks near the board’s edge. Here’s how to set it up:

  1. Define Edge Distance Rule: Building on the previous setup, set the overall clearance to 0.152mm and copper pour clearance to 0.5mm. Then, create a new rule with a 0.3mm distance from the copper to the board edge, naming it Keep-out.

  2. Specify Object Matching:

    • In the Where The First Object Matches window, select Net and choose GND from the dropdown.

    • In the Where The Second Object Matches window, select Layer and choose Keep-Out Layer.

  3. Set Rule Priorities: Click Priorities… to open the priority settings window and adjust rule priorities as needed.

202410281625333366.png

Indirect Copper Connections for Pads and Direct Connections for Vias

In copper pour design, different connection methods can be set for pads and vias. For example, pads can use indirect connections, while vias can use direct connections. Follow these steps:

  1. Default Copper Pour Connection Rule: Open the PCB Rules and Constraints Editor using “D” + “R”. By default, copper pour uses indirect connections, but you can adjust the trace width if needed.

  2. Create a New Rule for Via Connections: Right-click on Polygon Connect and select New Rule.

  3. Set Object Query: In the Where The First Object Matches window, select Advanced (Query), click Query Helper…, then type “isv…” to auto-select IsVia.

  4. Set Direct Connect for Vias: Select Direct Connect for vias and name the rule Via. 

202410281625343166.png

General Direct Copper Connection with Select Components Using Indirect Connections

For ease of maintenance or to improve soldering quality, you may want to set some components to use indirect connections while using direct connections for the overall copper pour. Here’s how to set it up:

  1. Set General Connection Method: Following the previous steps, create a rule to set direct connections as the default for the copper pour.

  2. Set Specific Component to Indirect Connection: For example, to set component JK1 to indirect connection, create a new rule. In the Where The First Object Matches window, choose Advanced (Query), click Query Helper…, type “inc…” to auto-select InComponent, then enter “j…” and choose JK1 from the dropdown.

  3. Name the Rule: Name this rule JK1.

  4. Adjust Priority Settings: Be sure to adjust the rule priority settings as needed to ensure proper rule application.

202410281625346808.png

By following these tips, you can optimize copper pour designs in Altium Designer, improving the PCB’s interference resistance and overall electrical performance. Proper use of clearance and rule settings not only increases circuit board reliability but also enhances the organization and maintainability of your design. We hope these practical tips will help you achieve efficient PCB design and improve project success.