The Tech Blog

I was doing some high speed PCB designing and thought AC coupling capacitors that are placed on high speed differential lines might be a good topic to discuss today. These are series capacitors you will see placed in USB 3/4 lines, PCI Express, HDMI etc.

Like any capacitor, at DC, it’s an open switch, at high frequency, it’s a dead short. Why do you need it? It blocks any DC voltage. Every differential link has two voltages: the desired differential swing (like +/-400mV) and an unwanted but expected common-mode voltage that both wires sit on, measured with respect to ground. The series capacitors block the DC part, letting each side of receiver/transmitter to coexist without any issues.

If there is any small ground offset(in mVs) between two sides, it would push a continuous long term DC current and waste power. Coupling caps block them. It also allows for hot plugging. Meaning if one side is powered, the other side is off, without any series capacitors, live driver will push DC current straight into pins that are still at 0 V, which is bad. By inserting series caps, you ensure no DC flows until both ends are fully powered and switching.

How to choose one? Most specs put cap values between 75nF and 220nF. With the 100Ω termination, that puts the high-pass freq in the tens of kilohertz, well under the spec to pass gigabits of data. I usually prefer using 0201 type capacitors, purely because they are small(low inductance) and they fit the differential pair lines width without majorly spacing it out. Placement matters. I place one cap in each leg, side by side, same orientation, pads inline, so the pair runs straight through. Keep stubs under half a millimetre and return to 100 Ω within a millimetre. Most spec/chips will tell you what you need to do.

Please take care of them while routing. They look tiny but if you get their placement or value wrong and your gigabit link will fail. It’s hard to debug them unless you have some high-end oscilloscopes. So treat them well.

Some of you might have seen these in PCBs. Let’s discuss in detail today.

In PCB manufacturing, during the final plating, the bare panel sits in an acid bath and a direct current pushes coats Copper on every exposed metal area on the PCB. Pads, vias and any existing copper act like little magnets. Areas that already have a lot of copper pull harder, empty laminate pulls less. Thick spots get thicker, thin spots remain thin. This is a problem in some cases like the via holes where you will have thickness difference, which in turn can cause signal integrity issues when high speed signals travel through them.

Copper thieving is done to fix this issue. Designers/Manufacturers put small, unconnected dots or rectangles into the blank places on the outer layers of the PCB. These islands are supposed to “steal” a part of the current from certain regions. Current density flattens out, so the whole panel plates at the same pace. This means uniform via walls and traces etch to the correct width/depth.

Do not confuse thieving with copper balancing, though. Balancing is a layout stage move where you mirror large ground pours across all layers so the stack-up expands and cools evenly during lamination and soldering. Thieving lives only on the two plated outer layer (inner layers are etched, not electro-plated). Balancing protects the overall PCB structure and prevents wrapage, while thieving is about fine-tuning in certain surface regions.

If you implement thieving, please remember to keep these islands some distance away from pads/high speed traces or antennas as they are usually not connected to avoid any unwanted coupling. Some folks do connect it to the ground layer with a few vias. So next time when you see some pretty rectangle islands or dots in the design, you will know it’s not there only for making it look nice, they do it to improve the manufacturing yield of PCBs.