I’ve observed numerous 2-layer PCBs with ground pours on both the top and bottom layers, prompting me to inquire about the rationale behind this practice. Wouldn’t it be more advantageous to utilize the top layer for power and signals, reserving the bottom layer for the ground? This approach could streamline routing and leverage the capacitance between the planes. What are your thoughts on this strategy?
Oh what a great question! How you approach this would depend on your circuit. Let’s say you have some 12 bit ADC’s in your circuit. They might have some millivolt signals going into them and in that case having ground pours all around helps isolate and shield those traces. On the other hand, if you had some 50 ohm single ended traces, you would want ground underneath them to create a transmission line, and would want to avoid ground pours being too close to the signal traces causing capacitive loading. Many of the 2 layer designs I’ve done had power on the bottom and ground pour on the top, but either way the power and ground form a capacitor and help alleviate noise from the board. Bottom line, think of what the signals are doing and the best environment for them prior to making those decisions.
1 Like
I will address your question from a different perspective. Designing 2-layer boards is a bad design and creates many issues with today’s technology. Perhaps for very low-speed signals or DC-based maybe. What we know currently is the effect of Energy moving into the space of the Live Trace and its return. Power is not return, but the lower potential, call it ground. So what’s important is the Energy moving in the dielectric (space) in a board. So to answer your question, we need to think what is your circuit. Some folks have ground under and poor power on top and others have power under poor ground on top to balance the to layers, and if the board is small, there is almost no interlayer capacitance because the separation might be very far away. So the poring just creates problems rather than solves them. but the reality is Energy moves and travels from point A to point be through space. This concept is well understood by Microwavewave engineers because we are used to dealing with waves, e, and H fields. Please play this video and well explained and will enlight more hw_introisledungeon1e_h_all_120 (youtube. com)
1 Like
Good layout and proper grounding are often misunderstood, leading to misconceptions. Typically, there’s rarely a strong case for using both the top and bottom layers of a two-layer PCB for ground. In two-layer designs, typically place as many interconnects as possible on the top layer since that’s where the component pins are already located. While careful part placement can help, it’s usually impossible to route everything on one layer. In such cases, reserve the bottom layer mostly for ground and use it sparingly for short “jumper” traces to complete the routing. The key is to keep these jumpers short and spaced apart so they don’t interfere too much with the ground plane.
When evaluating how well your ground plane is preserved, it’s more about the largest uninterrupted section than the total number of holes. A few small 200-mil traces scattered across the bottom layer won’t disrupt the ground plane much, but if you group those traces into one large island an inch across, you’ll create a significant disturbance. The goal is to allow the ground to flow around any disruptions smoothly.
When using an auto-router, set a high routing cost for the bottom layer and keep the via penalty low. This will naturally push most of the routing to the top. Unfortunately, auto-routers tend to clump jumpers together, which you’ll have to manually separate to avoid creating large gaps in the ground plane. Tools like Eagle’s “hugging” parameter can help, but even then, you’ll likely need to clean up the results after the auto-routing process. Sometimes, a small tweak in component placement can eliminate the need for a jumper entirely.
As for power planes, they’re often unnecessary in most designs. Power can be routed like any other signal, but you should pay attention to voltage drops due to trace resistance, especially if the circuit handles significant current. Even 1 oz copper traces have fairly low resistance, so making the power traces wider—around 20 mils instead of the typical 8 mils for signals—can usually handle the current without issue.
The common misconception is focusing too much on the AC impedance of power traces, but that’s less critical in practice. This is because each component is locally bypassed to the ground plane at its power pin, so the high-frequency current doesn’t travel across the entire plane. To minimize RF emissions, bypass capacitors should be placed directly between the power and ground pins of each part, with a via connecting the ground pin to the ground plane right at that spot. Avoid using separate vias for the ground side of the bypass cap—this keeps the high-frequency loop small and clean, improving overall circuit performance.
1 Like
Having a power plane on the top and a ground plane on the bottom of the PCB results in very little capacitance. Using the formula for capacitance:
C=k⋅ϵo⋅(A/d)
Where:
- k is the relative permittivity (around 4.5 for FR4),
- ϵo is the permittivity of free space (8.85 pF/m),
- A is the area in square meters,
- d is the separation distance in meters.
For example, with a Eurocard-sized PCB (160 mm × 100 mm) and a board thickness of 1.6 mm, the capacitance would be:
C=4.5⋅8.85 pF/m⋅(0.016 m2/0.0016 m) =400pF
This is very low compared to what you can achieve with decoupling capacitors, which provide significantly higher capacitance. When properly decoupled, it doesn’t matter whether you use ground or power for your copper pours at high frequencies—they essentially behave the same.
Ground is usually preferred for copper pours because it typically has the most connections. It also simplifies linking isolated copper pours on the top layer to those on the bottom layer.
1 Like
Using a top power plane can greatly accelerate routing when compared to having ground planes on both the top and bottom layers.
For simple two-layer boards, where all components are placed on the top layer, one effective routing strategy involves the following steps:
- Assign the bottom layer as a ground plane.
- Use vias to connect the ground pads of components on the top layer to the ground plane.
- Designate the top layer as a power plane.
This approach quickly eliminates many air wires, streamlining the routing process.
Afterward, focus on routing the critical data paths. Additionally, incorporating a plane on both layers helps reduce the amount of etchant used during manufacturing. Over time and across many boards, this can contribute to a reduction in chemical waste, promoting more sustainable PCB production.
1 Like