The Importance of Copper Pour in Empty Areas on PCBs

Having too much empty space without copper in a PCB design can have negative effects on manufacturing and the quality of the final product. Placing copper pour means filling unused space on a PCB with planar copper. It is an important part of PCB design and all major PCB design software is able to automatically place copper pour. Copper pour helps build EMC by lowering ground impedance, increasing power efficiency by reducing voltage drops, and mitigating EMI by shrinking loop areas.

JLCPCB has five self-owned intelligent production bases and has been using industry-leading equipment and raw materials to produce high-quality PCBs. JLCPCB has excellent control over all production links in PCB. In this article, we will take a peek through the JLCPCB factory, explore how PCBs are plated and etched, and see why it is important to have copper pour in unused board areas and also what needs to be noted when using copper pour.

You might ask: Doesn't leave unused areas blank save cost, since we are using less copper? The answer is: Yes, but having copper in empty areas benefits quality and yield and these are more important.

Unused areas left blank

Unused areas filled with copper pour

Outer Layer copper pour: 2- and Multi-layer Boards

Once dry film has been applied to the boards, they are placed in a plating solution to undergo electroplating using a fixed current.

Imaged PCBs ready for electroplating

Exposed copper that is not covered by the dry film will grow in thickness from copper in the solution under the effect of the current.

PCBs undergoing electroplating in an electrolyte bath

During this process, the amount of exposed copper area will affect the distribution of the electric current. The current acts more evenly on large areas of copper, and this is why large copper pour is recommended in PCB designs.

Large areas of copper exposed for plating

On the contrary, if the exposed copper areas are small or not evenly distributed on the PCB, they will experience different amounts of current and eventually have different thicknesses, with higher current resulting in a thicker plating. This can cause a nominally 1 oz board to have 2 oz copper thickness.

Not enough copper exposed during plating

The chemical process of electroplating

When two traces with very little spacing (e.g. 4 or 5 mil) and no surrounding copper undergo electroplating, they grow so thick that the dry film between them becomes difficult to remove before etching. This causes unwanted copper to remain between the traces, potentially leading to short circuits.

Dry film remains between two closely spaced traces

Solution

To ensure the quality, avoid creating "standalone" traces as much as possible in your design, and lay the copper pour on the entire board as much as possible. If some of the "standalone" traces can't be laid with copper pour, design the gap between the traces as wide as possible. The following are some examples of problematic designs and their improved versions.

Copper pour has only partial coverage:

Before Improvement

After Improvement

No copper pour at all:

Before Improvement

After Improvement

Inner Layer copper pour: Multi-layer Boards

Multi-layer PCBs are laminated by cutting prepreg to the correct size, placing it between two core layers or one core layer and one copper sheet layer, and subjecting the assembly to high temperature and pressure to melt and cure the resin within the prepreg in order to bond the layers together.

Prepreg

Inner layer core

Laminate

1) If a copper layer has large blank areas, resin on the prepreg will have to spread out to fill the copper-free zone. This can cause thinner-than-usual PCBs, folds and creases in the copper, voids in the resin, and potentially layer separation.

A fold in a copper layer

Voids in a resin layer, visible from the white marks

Design example:

Before Improvement

After Improvement

2) If the inner layer area of the goldfinger is very empty, the goldfinger area will be thinner than expected and this can cause poor contact between the PCB and the mating connector slot, etc.

1.6 mm nominal, 1.41 mm measured

Before: no copper pour in inner layer area of the goldfingers

After Improvement

For PCBs with gold fingers: copper pour must be applied in the inner layer area of the goldfingers because those areas have stricter thickness requirements. When ordering, make sure to select a stack-up that has sufficient nominal finished thickness, and avoid stack-ups whose thickness is near your acceptable lower limit.

Below is the discussion about notes on using copper pour. For multi-layer boards, copper pour in the empty area of the inner layer is mainly to increase the copper area and reduce the resin spread out area, so as to ensure the reliability of lamination and the thickness tolerance of the finished board. The purpose of copper pour in the empty area of the outer layer is mainly to even the electroplating current, avoid the risk of short circuits and thin lines caused by over-etching, and make the surface copper thickness more uniform.

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 neighbouring 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.

Pad Type	Direct Connection	Thermal Relief
Example
Description	A pad which is fully connected to the plane dissipates heat quickly during soldering, requiring longer soldering times and higher temperatures. This is bad because prolonged exposure to high temperature can cause the copper plane to deform.	Better design: Use thermal reliefs around pads within copper planes. The black areas are gaps in the copper. Both the spoke width (A) and gap (B) should be wider than 0.25 mm. Thermal reliefs reduce heat dissipation and improve soldering quality due to less wasted energy.

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 an 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 increase current capacity but also reduce 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 pour. 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 pours instead of hatched ones where possible.

Pour Type	None	Hatched	Solid
Image
Description	Not recommended. Having no copper pour can cause warping and other defects.	Not recommended. Hatched patterns can cause film cracks and thus quality concerns. Keep gap (A) and width (B) above 0.25 mm if hatched copper is required.	Ideal design: Fill empty areas with solid copper. Keep at least 0.2 mm clearance from traces and pads, or 0.5 mm for high-speed traces.

GET FREE QUOTE>>

Copper Fills on Inner Layers

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

Coverage	100%	85%
Photo Example

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 pressurised 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.

Material	Prepreg	Inner Core	Laminate
Photo

Design issue: Low copper coverage on inner layers means resin from the prepreg has to spread out more to fill the copper-free zone. 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.

Defect	Copper Layer “Wrinkles”	Resin Voids
Photo

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.

Design	Before	Improved
Copper Layer

Calculating Total Laminate and Finished 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).

Design Guidelines Summary

1. Don’t leave any PCB area blank without copper. Fill these areas with copper pour.

2. If copper pour is not possible, then traces should be designed assuming 2 oz copper weight and 8 mil minimum spacing(trace to trace, trace to pad, pad to pad).

3. Copper pour should have plenty of clearance from functional traces and pads, ideally more than 0.5 mm. Avoid using hatched copper patterns, especially small grid sizes; prefer solid pours instead.

4. Copper pour must be present in all the inner layers of gold fingers to avoid insufficient board thickness. Avoid stack-ups with thinner finished thicknesses.

5. Around PCB antennas, copper pour should be designed according to specific product requirements to avoid interfering with the antenna’s operation.

Note: The importance of JLCPCB adding copper pour

For multi-layer PCBs, JLCPCB may add 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.

JLCPCB regards driving tech innovation as its responsibility and keeps striving to provide customers with a wider selection of PCB manufacturing. That's not all, JLCPCB also provides one-stop PCBA from ordering quality PCBs to sourcing 1 Million+ genuine electronic components and to assembling your PCBs with state-of-the-art SMT machines. Sign up at JLCPCB official website to get up to $60 new user coupons, starting your PCB journey from here!