PCB Copper Pour Basics

What is Copper Pour in PCB Design?

Copper pour refers to the technique of filling unused areas of a PCB's copper layers with solid copper planes. These planes are connected to power or ground nets, creating a continuous conductive path. Copper pour is typically used in the power and ground planes, as well as in signal layers for specific purposes.

Purpose of Copper Pour:

Ground Plane: Copper pour can create a solid ground plane, providing a low impedance return path for signals and reducing electromagnetic interference (EMI).

Power Plane: Copper pour can be used as a power plane to distribute power evenly across the PCB, minimizing voltage drops and enhancing power stability.

Heat Dissipation: Copper pour acts as a heat sink, spreading and dissipating heat generated by power components, thus preventing overheating and ensuring the reliability of the PCB.

Benefits of Copper Pour:

Enhanced Signal Integrity: By reducing ground loops, noise, and interference, copper pour helps maintain signal integrity and minimize signal degradation.

Improved Thermal Management: Copper pour enhances heat dissipation, preventing hotspots and ensuring optimal operating temperatures for components.

Copper Savings: Effective utilization of copper pour can reduce the need for additional traces and increase copper utilization efficiency, resulting in cost savings.

Implementation of Copper Pour:

Placing a copper pour means filling unused space on a PCB with planar copper. They are an important part of PCB design and all major PCB design software are able to automatically place them. Copper pour helps build EMC by lowering ground impedance, increase power efficiency by reducing voltage drops, and mitigate EMI by reducing loop areas.

Use Thermal Relief Pads Within Copper Pour

Copper is very thermally conductive (approx. 380W/(m·K)). Because of this, if a pad is fully connected on all sides to its neighboring copper plane, heat will dissipate away extremely quickly during soldering, causing soldering issues. “Thermal relief” pads are used to reduce heat dissipation and help with soldering.

Hatched and Solid Copper Pour

As we know, distributed capacitance of the traces on a PCB comes into play under high-frequency conditions. When the length of a trace is greater than 1/20 of the corresponding wavelength of the noise frequency, the trace acts as a antenna and transmits this noise into the surrounding space. Any copper pour which is poorly grounded will help further propagate this noise. Therefore, in high-frequency circuits, ground connections not only need electrical continuity, but must also be spaced less than λ/20. Vias on traces can help achieve “good grounding” to the ground plane of multilayer boards. Properly designed copper planes not only increases current capacity but also reduces EMI.

There are generally two styles of copper pour: solid and hatched. Solid pours both increase current capacity and provide shielding, but may cause warping and copper detachment when passed through wave soldering. This is alleviated by designing slots/openings into solid copper pours. On the other hand, hatched pours are mainly used for shielding and don’t have very high current carrying ability. Hatched pours may be beneficial for heat dissipation because they have reduced copper area. However, one downside to hatched pours is that the copper “segments” it consists of can increase EMI: when the length of these segments is similar to the electrical length of the circuit’s operating frequency, the circuit might not work at all due to the whole pour acting as many antennas all transmitting interfering signals. It’s best to choose the type of copper pour to fit the circuit on the PCB: use hatched pours for high-frequency circuits with EMI requirements, and solid pours for low-frequency or high-current circuits.

With modern PCB designs demanding more precision and quality, all major PCB manufacturers have abandoned the low-cost wet film process and have adopted the superior dry film process. Hatched copper pour can cause the film to crack with dry film processes, so it’s recommended to use solid pour instead of hatched ones where possible.

Copper Fills on Inner Layers

Copper coverage: the area of copper remaining on an inner layer after etching relative to the total board area.

Laminating: Prepreg is cut to the appropriate size then placed between inner layer cores or between a core and a copper sheet. The layered stack (laminate) is heated and pressurized to melt the resin content in the prepreg layers. The resin flows to fill the areas without copper on the adjacent layers, and bonds the layers together once cooled.

Design issue: Low copper coverage means resin from the prepreg has to spread out more to fill the place of the missing copper. Consequences include a thinner board than expected, folds/wrinkles in copper layers, voids in the resin, and potential layer separation due to lack of resin.

Design suggestion: Place copper pour in empty areas of the board where possible. Keep at least 0.5 mm clearance from high-speed signal traces.

Calculating Total Laminate and Board Thickness

Theoretical laminate thickness

= outer copper + cured prepreg + core

= (0.7×2) + (4.54+4.48) + (1.2+44.84+1.2) = 57.66 mil = 1.46 mm.

Theoretical board thickness

= soldermask + plated outer copper +  cured prepreg + core

= (1×2) + (1.4×2) + (4.54+4.48) + (1.2+44.84+1.2) = 61.06 mil = 1.55 mm.

Where the cured prepreg thickness

= Uncured prepreg thickness – thickness to be filled by resin on adjacent core layers

= Uncured prepreg thickness – ((1 – copper coverage) × copper thickness)

An example stack-up is described in the table below.

Taking layers 1 and 2 as example:

• Uncured prepreg thickness = 4.72 mil, layer 2 copper coverage = 85%, inner layer copper weight = 1 oz,
• Cured prepreg thickness = 4.72 – ((1 – 85%) × 1.2) = 4.54 mil.

Although the nominal 1 oz copper thickness is 35 μm, due to losses during pre-processing and browning, the actual thickness is 30 μm (1.2 mil).

Copper Pour Be Added To Panels by JLCPCB

JLCPCB adds copper pour to panels on both inner and outer layers to avoid defects caused by large empty spaces such as low board thickness and uneven plating. Copper pour will only be added to handling strips, bridge pieces and other areas outside PCB units. No copper will be added inside the useful PCBs. Clearance will be added around fiducials, mechanical holes, mouse bites, and V-cuts.

GET FREE QUOTE>>